Next: Obtaining Gmsh, Previous: (dir), Up: (dir) [Contents][Index]
Christophe Geuzaine and Jean-François Remacle
Gmsh is an automatic 3D finite element mesh generator with build-in pre- and post-processing facilities. This is the Gmsh Reference Manual for Gmsh 4.8.4 (development version) (May 12, 2023).
t1
: Geometry basics, elementary entities, physical groupst2
: Transformations, extruded geometries, volumest3
: Extruded meshes, ONELAB parameters, optionst4
: Built-in functions, holes in surfaces, annotations, entity colorst5
: Mesh sizes, macros, loops, holes in volumest6
: Transfinite meshest7
: Background meshest8
: Post-processing and animationst9
: Pluginst10
: Mesh size fieldst11
: Unstructured quadrangular meshest12
: Cross-patch meshing with compoundst13
: Remeshing an STL file without an underlying CAD modelt14
: Homology and cohomology computationt15
: Embedded points, lines and surfacest16
: Constructive Solid Geometry, OpenCASCADE geometry kernelt17
: Anisotropic background mesht18
: Periodic meshest19
: Thrusections, fillets, pipes, mesh size from curvaturet20
: STEP import and manipulation, geometry partitioningt21
: Mesh partitioningx1
: Geometry and mesh datax2
: Mesh import, discrete entities, hybrid models, terrain meshingx3
: Post-processing data import: list-basedx4
: Post-processing data import: model-basedgmsh
: top-level functionsgmsh/option
: option handling functionsgmsh/model
: model functionsgmsh/model/mesh
: mesh functionsgmsh/model/mesh/field
: mesh size field functionsgmsh/model/geo
: built-in CAD kernel functionsgmsh/model/geo/mesh
: built-in CAD kernel meshing constraintsgmsh/model/occ
: OpenCASCADE CAD kernel functionsgmsh/model/occ/mesh
: OpenCASCADE CAD kernel meshing constraintsgmsh/view
: post-processing view functionsgmsh/plugin
: plugin functionsgmsh/graphics
: graphics functionsgmsh/fltk
: FLTK graphical user interface functionsgmsh/onelab
: ONELAB server functionsgmsh/logger
: information logging functionsNext: Copying conditions, Previous: Gmsh, Up: Gmsh [Contents][Index]
The source code and various pre-compiled versions of Gmsh (for Windows, Mac and Unix) can be downloaded from https://gmsh.info. Gmsh is also directly available in pre-packaged form in various Linux and BSD distributions (Debian, Ubuntu, FreeBSD, ...).
If you use Gmsh, we would appreciate that you mention it in your work by citing the following paper: “C. Geuzaine and J.-F. Remacle, Gmsh: a three-dimensional finite element mesh generator with built-in pre- and post-processing facilities. International Journal for Numerical Methods in Engineering, Volume 79, Issue 11, pages 1309-1331, 2009”. A preprint of that paper as well as other references and the latest news about Gmsh development are available on https://gmsh.info.
Next: Overview, Previous: Obtaining Gmsh, Up: Gmsh [Contents][Index]
Gmsh is “free software”; this means that everyone is free to use it and to redistribute it on a free basis. Gmsh is not in the public domain; it is copyrighted and there are restrictions on its distribution, but these restrictions are designed to permit everything that a good cooperating citizen would want to do. What is not allowed is to try to prevent others from further sharing any version of Gmsh that they might get from you.
Specifically, we want to make sure that you have the right to give away copies of Gmsh, that you receive source code or else can get it if you want it, that you can change Gmsh or use pieces of Gmsh in new free programs, and that you know you can do these things.
To make sure that everyone has such rights, we have to forbid you to deprive anyone else of these rights. For example, if you distribute copies of Gmsh, you must give the recipients all the rights that you have. You must make sure that they, too, receive or can get the source code. And you must tell them their rights.
Also, for our own protection, we must make certain that everyone finds out that there is no warranty for Gmsh. If Gmsh is modified by someone else and passed on, we want their recipients to know that what they have is not what we distributed, so that any problems introduced by others will not reflect on our reputation.
The precise conditions of the license for Gmsh are found in the General Public License that accompanies the source code (see License). Further information about this license is available from the GNU Project webpage https://www.gnu.org/copyleft/gpl-faq.html. Detailed copyright information can be found in Copyright and credits.
If you want to integrate parts of Gmsh into a closed-source software, or want to sell a modified closed-source version of Gmsh, you will need to obtain a different license. Please contact us directly for more information.
Next: How to read this reference manual?, Previous: Copying conditions, Up: Gmsh [Contents][Index]
Gmsh is a three-dimensional finite element mesh generator with a build-in CAD engine and post-processor. Its design goal is to provide a fast, light and user-friendly meshing tool with parametric input and advanced visualization capabilities.
Gmsh is built around four modules: geometry, mesh, solver and post-processing. All geometrical, mesh, solver and post-processing instructions are prescribed either interactively using the graphical user interface (GUI) or in text files using Gmsh’s own scripting language. Interactive actions generate language bits in the input files, and vice versa. A programming API is also available, for integrating Gmsh in your own C++, C, Python or Julia code: see Gmsh API. A brief description of the four modules is given hereafter.
Next: Mesh: finite element mesh generation, Previous: Overview, Up: Overview [Contents][Index]
A model in Gmsh is defined using its Boundary Representation (BRep): a volume is bounded by a set of surfaces, a surface is bounded by a series of curves, and a curve is bounded by two end points. Model entities are topological entities, i.e., they only deal with adjacencies in the model, and are implemented as a set of abstract topological classes. This BRep is extended by the definition of embedded, or internal, model entities: internal points, edges and surfaces can be embedded in volumes; and internal points and curves can be embedded in surfaces.
The geometry of model entities can be provided by different CAD kernels. The two default kernels interfaced by Gmsh are the “Built-in” kernel and the “OpenCASCADE” kernel. Gmsh does not translate the geometrical representation from one kernel to another, or from these kernels to some neutral representation. Instead, Gmsh directly queries the native data for each CAD kernel, which avoids data loss and is crucial for complex models where translations invariably introduce issues linked to slightly different representations.
Gmsh’s scripting language and the Gmsh API allow to parametrize all model entities. The entities can either be built in a “bottom-up” manner (first points, then curves, surfaces and volumes) or in a “Constructive Solid Geometry” fashion (solids on which boolean operations are performed). Both methodologies can also be combined. Finally, groups of model entities (called “physical groups”) can be defined, based on the elementary geometric entities.
Next: Solver: external solver interface, Previous: Geometry: model entity creation, Up: Overview [Contents][Index]
A finite element mesh of a model is a tessellation of its geometry by simple geometrical elements of various shapes (in Gmsh: lines, triangles, quadrangles, tetrahedra, prisms, hexahedra and pyramids), arranged in such a way that if two of them intersect, they do so along a face, an edge or a node, and never otherwise. This defines a so-called “conformal” mesh. Gmsh implements several algorithms to generate such meshes automatically. All the meshes produced by Gmsh are considered as “unstructured”, even if they were generated in a “structured” way (e.g., by extrusion). This implies that the mesh elements are completely defined simply by an ordered list of their nodes, and that no predefined ordering relation is assumed between any two elements.
In order to guarantee the conformity of the mesh, mesh generation is performed in a bottom-up flow: curves are discretized first; the mesh of the curves is then used to mesh the surfaces; then the mesh of the surfaces is used to mesh the volumes. In this process, the mesh of an entity is only constrained by the mesh of its boundary, unless entities of lower dimensions are explicitly embedded in entities of higher dimension. For example, in three dimensions, the triangles discretizing a surface will be forced to be faces of tetrahedra in the final 3D mesh only if the surface is part of the boundary of a volume, or if that surface has been explicitly embedded in the volume. This automatically ensures the conformity of the mesh when, for example, two volumes share a common surface. Every meshing step is constrained by a mesh “size field”, which prescribes the desired size of the elements in the mesh. This size field can be uniform, specified by values associated with points in the geometry, or defined by general “fields” (for example related to the distance to some boundary, to a arbitrary scalar field defined on another mesh, etc.): see Specifying mesh element sizes. For each meshing step, all structured mesh directives are executed first, and serve as additional constraints for the unstructured parts.
Next: Post-processing: scalar, vector and tensor field visualization, Previous: Mesh: finite element mesh generation, Up: Overview [Contents][Index]
Gmsh implements a ONELAB (http://onelab.info) server to pilot external solvers (called “clients”). The ONELAB interface allows to call such clients and have them share parameters and modeling information. The implementation is based on a client-server model, with a server-side database and local or remote clients communicating in-memory or through TCP/IP sockets. Contrary to most solver interfaces, the ONELAB server has no a priori knowledge about any specifics (input file format, syntax, ...) of the clients. This is made possible by having any simulation preceded by an analysis phase, during which the clients are asked to upload their parameter set to the server. The issues of completeness and consistency of the parameter sets are completely dealt with on the client side: the role of ONELAB is limited to data centralization, modification and re-dispatching.
Examples on how to interface solvers are available in the source distribution (see utils/solvers). A full-featured solver interfaced in this manner is GetDP (https://getdp.info), a general finite elements solver using mixed finite elements.
Using the Gmsh API, Gmsh can also be embedded directly in your own solver, and ONELAB parameters can be used to interactively drive it. Examples on how to embed Gmsh in your solver, and build a custom graphical user interface to control it, are available in demos/api. See in particular custom_gui.py and custom_gui.cpp.
Next: What Gmsh is pretty good at …, Previous: Solver: external solver interface, Up: Overview [Contents][Index]
Gmsh can load and manipulate multiple post-processing scalar, vector or tensor fields along with the geometry and the mesh. Such fields, together with visualization options, are called “post-processing views” (or simply “views”). Scalar views can be represented by iso-curves, iso-surfaces or color maps, while vector views can be represented by three-dimensional arrows or displacement maps. Post-processing functions include section computation, offset, elevation, boundary and component extraction, color map and range modification, animation, vector graphic output, etc. All the post-processing options can be accessed either interactively, through the input script files or through the API. Various operations on the post-processing data can also be performed through plugins (see Post-processing plugins).
Next: … and what Gmsh is not so good at, Previous: Post-processing: scalar, vector and tensor field visualization, Up: Overview [Contents][Index]
Here is a tentative list of what Gmsh does best:
t8
: Post-processing and animations);
Next: Bug reports, Previous: What Gmsh is pretty good at …, Up: Overview [Contents][Index]
Here are some known weaknesses of Gmsh:
If you have the skills and some free time, feel free to join the project: we gladly accept any code contributions (see Information for developers) to remedy the aforementioned (and all other) shortcomings!
Previous: … and what Gmsh is not so good at, Up: Overview [Contents][Index]
Please file issues on https://gitlab.onelab.info/gmsh/gmsh/issues. Provide as precise a description of the problem as you can, including sample input files that produce the bug. Don’t forget to mention both the version of Gmsh and the version of your operation system (see Command-line options to see how to get this information).
See Frequently asked questions, and the bug tracking system to see which problems we already know about.
Next: Running Gmsh on your system, Previous: Overview, Up: Gmsh [Contents][Index]
Gmsh can be used at three levels:
You can skip most of this reference manual if you only want to use Gmsh at the first level (i.e., interactively with the GUI). Just read the next chapter (see Running Gmsh on your system) to learn how to launch Gmsh on your system, then go experiment with the GUI and the tutorial files (see Tutorial) provided in the distribution. Screencasts that show how to use the GUI are available here: https://gmsh.info/screencasts/.
The aim of the reference manual is to explain everything you need to use Gmsh at the second level, i.e., using the built-in scripting language. A Gmsh script file is an ASCII text file that contains instructions in Gmsh’s built-in scripting language. Such a file is interpreted by Gmsh’s parser, and can be given any extension (or no extension at all). By convention, Gmsh uses the .geo extension for geometry scripts, and the .pos extension for parsed post-processing datasets. Once you master the tutorial (read the source files: they are heavily commented!), start reading chapter General tools, then proceed with the next four chapters, which detail the syntax of the geometry, mesh, solver and post-processing scripting commands. You will see that most of the interactive actions in the GUI have a direct equivalent in the scripting language. If you want to use Gmsh as a pre- or post-processor for your own software, you will also want to learn about the non-scripting input/output files that Gmsh can read/write. In addition to Gmsh’s native “MSH” file format (see File formats), Gmsh can read/write many standard mesh files, depending on how it was built: check the ‘File->Export’ menu for a list of available formats.
Finally, to use Gmsh at the third level (i.e., to link the Gmsh library with your own code), you will need to learn the Gmsh Application Programming Interface (API). This API is available in C++, C, Python and Julia, and is fully documented in Gmsh API.
Previous: How to read this reference manual?, Up: How to read this reference manual? [Contents][Index]
Here are the rules we tried to follow when writing this reference manual. Note that metasyntactic variable definitions stay valid throughout the manual (and not only in the sections where the definitions appear).
this
.
:
) after a metasyntactic variable separates the variable
from its definition.
<
>
pairs.
|
.
Next: General tools, Previous: How to read this reference manual?, Up: Gmsh [Contents][Index]
Next: Non-interactive mode, Previous: Running Gmsh on your system, Up: Running Gmsh on your system [Contents][Index]
To launch Gmsh in interactive mode, just double-click on the Gmsh icon, or type
> gmsh
at your shell prompt in a terminal. This will open the main Gmsh window, with a tree-like menu on the left, a graphic area on the right, and a status bar at the bottom. (You can detach the tree menu using ‘Window->Attach/Detach Menu’.)
To open the first tutorial file (see Tutorial), select the ‘File->Open’ menu, and choose t1.geo. When using a terminal, you can specify the file name directly on the command line, i.e.:
> gmsh t1.geo
To perform the mesh generation, go to the mesh module (by selecting ‘Mesh’ in the tree) and choose the dimension (‘1D’ will mesh all the curves; ‘2D’ will mesh all the surfaces—as well as all the curves if ‘1D’ was not called before; ‘3D’ will mesh all the volumes—and all the surfaces if ‘2D’ was not called before). To save the resulting mesh in the current mesh format click on ‘Save’, or select the appropriate format and file name with the ‘File->Export’ menu. The default mesh file name is based on the name of the current active model, with an appended extension depending on the mesh format1.
To create a new geometry or to modify an existing geometry, select ’Geometry’ in the tree. For example, to create a spline, select ‘Elementary entities’, ‘Add’, ‘New’ and ‘Spline’. You will then be asked to select a list of points, and to type e to finish the selection (or q to abort it). Once the interactive command is completed, a text string is automatically added at the end of the current script file. You can edit the script file by hand at any time by pressing the ‘Edit’ button in the ‘Geometry’ menu and then reloading the model by pressing ‘Reload’. For example, it is often faster to define variables and points directly in the script file, and then use the GUI to define the curves, the surfaces and the volumes interactively.
Several files can be loaded simultaneously in Gmsh. When specified on
the command line, the first one defines the active model and the others
are ‘merged’ into this model. You can merge such files with the
‘File->Merge’ menu. For example, to merge the post-processing views
contained in the files
view1.pos
and
view5.msh
together with the geometry of the first tutorial t1
: Geometry basics, elementary entities, physical groups, you can type
the following command:
> gmsh t1.geo view1.pos view5.msh
In the Post-Processing module (select ‘Post-Processing’ in the tree), three items will appear, respectively labeled ‘A scalar map’, ‘Nodal scalar map’ and ‘Element 1 vector’. In this example the views contain several time steps: you can loop through them with the small “remote-control” icons in the status bar. A mouse click on the view name will toggle the visibility of the selected view, while a click on the arrow button on the right will provide access to the view’s options.
Note that all the options specified interactively can also be directly specified in the script files. You can save the current options of the current active model with the ‘File->Save Model Options’. This will create a new option file with the same filename as the active model, but with an extra .opt extension added. The next time you open this model, the associated options will be automatically loaded, too. To save the current options as your default preferences for all future Gmsh sessions, use the ‘File->Save Options As Default’ menu instead. Finally, you can also save the current options in an arbitrary file by choosing the ‘Gmsh options’ format in ‘File->Export’.
For more information about available options (and how to reset them to their default values), see Options. A full list of options with their current values is also available in the ‘Help->Current Options’ menu.
Next: Command-line options, Previous: Interactive mode, Up: Running Gmsh on your system [Contents][Index]
Gmsh can be run non-interactively in ‘batch’ mode, without GUI2. For example, to mesh the first tutorial in batch mode, just type:
> gmsh t1.geo -2
To mesh the same example, but with the background mesh available in the file bgmesh.pos, type:
> gmsh t1.geo -2 -bgm bgmesh.pos
For the list of all command-line options, see Command-line options. In particular, any complicated workflow can be written in a
.geo
file, and this file can be executed as a script using
> gmsh script.geo -
The script can contain e.g. meshing commands, like Mesh 3;
.
Next: Mouse actions, Previous: Non-interactive mode, Up: Running Gmsh on your system [Contents][Index]
(Related option names, if any, are given between parentheses)
Geometry:
-0
¶Output model, then exit
-tol value
¶Set geometrical tolerance (Geometry.Tolerance)
-match
¶Match geometries and meshes
Mesh:
-1, -2, -3
¶Perform 1D, 2D or 3D mesh generation, then exit
-save
¶Save mesh, then exit
-o file
¶Specify output file name
-format string
¶Select output mesh format: auto, msh1, msh2, msh22, msh3, msh4, msh40, msh41, msh, unv, vtk, wrl, mail, stl, p3d, mesh, bdf, cgns, med, diff, ir3, inp, ply2, celum, su2, x3d, dat, neu, m, key (Mesh.Format)
-bin
¶Create binary files when possible (Mesh.Binary)
-refine
¶Perform uniform mesh refinement, then exit
-barycentric_refine
¶Perform barycentric mesh refinement, then exit
-reclassify angle
¶Reclassify surface mesh, then exit
-reparam angle
¶Reparametrize surface mesh, then exit
-part int
¶Partition after batch mesh generation (Mesh.NbPartitions)
-part_weight [tri,quad,tet,hex,pri,pyr,trih] int
¶Weight of a triangle/quad/etc. during partitioning (Mesh.Partition[Tri,Quad,...]Weight)
-part_split
¶Save mesh partitions in separate files (Mesh.PartitionSplitMeshFiles)
-part_[no_]topo
¶Create the partition topology (Mesh.PartitionCreateTopology)
-part_[no_]ghosts
¶Create ghost cells (Mesh.PartitionCreateGhostCells)
-part_[no_]physicals
¶Create physical groups for partitions (Mesh.PartitionCreatePhysicals)
-part_topo_pro
¶Save the partition topology .pro file (Mesh.PartitionTopologyFile)
-preserve_numbering_msh2
¶Preserve element numbering in MSH2 format (Mesh.PreserveNumberingMsh2)
-save_all
¶Save all elements (Mesh.SaveAll)
-save_parametric
¶Save nodes with their parametric coordinates (Mesh.SaveParametric)
-save_topology
¶Save model topology (Mesh.SaveTopology)
-algo string
¶Select mesh algorithm: auto, meshadapt, del2d, front2d, delquad, pack, initial2d, del3d, front3d, mmg3d, hxt, initial3d (Mesh.Algorithm and Mesh.Algorithm3D)
-smooth int
¶Set number of mesh smoothing steps (Mesh.Smoothing)
-order int
¶Set mesh order (Mesh.ElementOrder)
-optimize[_netgen]
¶Optimize quality of tetrahedral elements (Mesh.Optimize[Netgen])
-optimize_threshold
¶Optimize tetrahedral elements that have a quality less than a threshold (Mesh.OptimizeThreshold)
-optimize_ho
¶Optimize high order meshes (Mesh.HighOrderOptimize)
-ho_[min,max,nlayers]
¶High-order optimization parameters (Mesh.HighOrderThreshold[Min,Max], Mesh.HighOrderNumLayers)
-clscale value
¶Set mesh element size factor (Mesh.MeshSizeFactor)
-clmin value
¶Set minimum mesh element size (Mesh.MeshSizeMin)
-clmax value
¶Set maximum mesh element size (Mesh.MeshSizeMax)
-clextend value
¶Extend mesh element sizes from boundaries (Mesh.MeshSizeExtendFromBoundary)
-clcurv value
¶Compute mesh element size from curvature, with value the target number of elements per 2*pi radians (Mesh.MeshSizeFromCurvature)
-aniso_max value
¶Set maximum anisotropy for bamg (Mesh.AnisoMax)
-smooth_ratio value
¶Set smoothing ration between mesh sizes at nodes of a same edge for bamg (Mesh.SmoothRatio)
-epslc1d value
¶Set accuracy of evaluation of mesh size field for 1D mesh (Mesh.LcIntegrationPrecision)
-swapangle value
¶Set the threshold angle (in degrees) between two adjacent faces below which a swap is allowed (Mesh.AllowSwapAngle)
-rand value
¶Set random perturbation factor (Mesh.RandomFactor)
-bgm file
¶Load background mesh from file
-check
¶Perform various consistency checks on mesh
-ignore_periocity
¶Ignore periodic boundaries (Mesh.IgnorePeriodicity)
Post-processing:
-link int
¶Select link mode between views (PostProcessing.Link)
-combine
¶Combine views having identical names into multi-time-step views
Solver:
-listen string
¶Always listen to incoming connection requests (Solver.AlwaysListen) on the given socket (uses Solver.SocketName if not specified)
-minterpreter string
¶Name of Octave interpreter (Solver.OctaveInterpreter)
-pyinterpreter string
¶Name of Python interpreter (Solver.OctaveInterpreter)
-run
¶Run ONELAB solver(s)
Display:
-n
¶Hide all meshes and post-processing views on startup (View.Visible, Mesh.[Points,Lines,SurfaceEdges,...])
-nodb
¶Disable double buffering (General.DoubleBuffer)
-numsubedges
¶Set num of subdivisions for high order element display (Mesh.NumSubEdges)
-fontsize int
¶Specify the font size for the GUI (General.FontSize)
-theme string
¶Specify FLTK GUI theme (General.FltkTheme)
-display string
¶Specify display (General.Display)
-camera
¶Use camera mode view (General.CameraMode)
-stereo
¶OpenGL quad-buffered stereo rendering (General.Stereo)
-gamepad
¶Use gamepad controller if available
Other:
-, -parse_and_exit
¶Parse input files, then exit
-new
¶Create new model before merge next file
-merge
¶Merge next files
-open
¶Open next files
-log filename
¶Log all messages to filename
-a, -g, -m, -s, -p
¶Start in automatic, geometry, mesh, solver or post-processing mode (General.InitialModule)
-pid
¶Print process id on stdout
-watch pattern
¶Pattern of files to merge as they become available (General.WatchFilePattern)
-bg file
¶Load background (image or PDF) file (General.BackgroundImageFileName)
-v int
¶Set verbosity level (General.Verbosity)
-string "string"
¶Parse command string at startup
-setnumber name value
¶Set constant or option number name=value
-setstring name value
¶Set constant or option string name=value
-nopopup
¶Don’t popup dialog windows in scripts (General.NoPopup)
-noenv
¶Don’t modify the environment at startup
-nolocale
¶Don’t modify the locale at startup
-option file
¶Parse option file at startup
-convert files
¶Convert files into latest binary formats, then exit
-nt int
¶Set number of threads (General.NumThreads)
-cpu
¶Report CPU times for all operations
-version
¶Show version number
-info
¶Show detailed version information
-help
¶Show command line usage
-help_options
¶Show all options
Next: Keyboard shortcuts, Previous: Command-line options, Up: Running Gmsh on your system [Contents][Index]
Highlight the entity under the mouse pointer and display its properties / Resize a lasso zoom or a lasso (un)selection
Rotate / Select an entity / Accept a lasso zoom or a lasso selection
Start a lasso zoom or a lasso (un)selection
Zoom / Unselect an entity / Accept a lasso zoom or a lasso unselection
Orthogonalize display
Pan / Cancel a lasso zoom or a lasso (un)selection / Pop-up menu on post-processing view button
Reset to default viewpoint
For a 2 button mouse, Middle button = Shift+Left button.
For a 1 button mouse, Middle button = Shift+Left button, Right button = Alt+Left button.
Previous: Mouse actions, Up: Running Gmsh on your system [Contents][Index]
(On Mac Ctrl is replaced by Cmd (the ‘Apple key’) in the shortcuts below.)
Go to previous time step
Go to next time step
Make previous view visible
Make next view visible
Reload geometry
Reload full project
Mesh lines
Mesh surfaces
Mesh volumes
Cancel lasso zoom/selection, toggle mouse selection ON/OFF
End/accept selection in geometry creation mode
Go to geometry module
Go to mesh module
Go to post-processing module
Abort selection in geometry creation mode
Go to solver module
Toogle x coordinate freeze in geometry creation mode
Toogle y coordinate freeze in geometry creation mode
Toogle z coordinate freeze in geometry creation mode
Bring all windows to front
Show geometry options
Show mesh options
Show general options
Show post-processing options
Show solver options
Show post-processing view plugins
Show post-processing view options
Move only along x coordinate in geometry creation mode
Move only along y coordinate in geometry creation mode
Move only along z coordinate in geometry creation mode
Enable full mouse selection
Attach/detach menu
Export project
Enter full screen
Show statistics window
Save model options
Show message console
Minimize window
Create new project file
Open project file
Quit
Rename project file
Save mesh in default format
Show clipping plane window
Show current options and workspace window
Save options as default
Show manipulator window
Show option window
Merge file(s)
Open next-to-last opened file
Show plugin window
Show visibility window
Loop through axes modes
Hide/show bounding boxes
Loop through predefined color schemes
Hide/Show element outlines for visible post-pro views
Change redraw mode (fast/full)
Hide/show all post-processing views
Hide/show all post-processing view scales
Hide/show geometry lines
Toggle visibility of all mesh entities
Hide/show all post-processing view annotations
Change projection mode (orthographic/perspective)
Hide/show geometry points
Loop through range modes for visible post-pro views
Hide/show geometry surfaces
Loop through interval modes for visible post-pro views
Hide/show geometry volumes
Enable/disable all lighting
Set X view
Set Y view
Set Z view
Set 1:1 view
Hide/show small axes
Hide/show mesh volume faces
Loop through predefined colormaps
Hide/show mesh surface faces
Hide/show mesh lines
Hide/show mesh nodes
Hide/show mesh surface edges
Same as Alt+t, but with numeric mode included
Hide/show mesh volume edges
Set -X view
Set -Y view
Set -Z view
Reset bounding box around visible entities
Sync scale between viewports
Next: Geometry module, Previous: Running Gmsh on your system, Up: Gmsh [Contents][Index]
This chapter describes the general commands and options that can be used in Gmsh’s script files. By “general”, we mean “not specifically related to one of the geometry, mesh, solver or post-processing modules”. Commands peculiar to these modules will be introduced in Geometry module, Mesh module, Solver module, and Post-processing module, respectively.
If you plan to use Gmsh through its API (see Gmsh API) instead of the built-in scripting language, you can skip this chapter entirely.
Next: Expressions, Previous: General tools, Up: General tools [Contents][Index]
Gmsh script files support both C and C++ style comments:
/*
and */
pairs is ignored;
//
is ignored.
These commands won’t have the described effects inside double quotes or inside keywords. Also note that ‘white space’ (spaces, tabs, new line characters) is ignored inside all expressions.
Next: Operators, Previous: Comments, Up: General tools [Contents][Index]
The two constant types used in Gmsh scripts are real and string (there is no integer type). These types have the same meaning and syntax as in the C or C++ programming languages.
Next: Character expressions, Previous: Expressions, Up: Expressions [Contents][Index]
Floating point expressions (or, more simply, “expressions”) are denoted by the metasyntactic variable expression (remember the definition of the syntactic rules in Syntactic rules used in the manual), and are evaluated during the parsing of the script file:
expression: real | string | string ~ { expression } string [ expression ] | # string [ ] | ( expression ) | operator-unary-left expression | expression operator-unary-right | expression operator-binary expression | expression operator-ternary-left expression operator-ternary-right expression | built-in-function | real-option | Find(expression-list-item, expression-list-item) | StrFind(char-expression, char-expression) | StrCmp(char-expression, char-expression) | StrLen(char-expression) | TextAttributes(char-expression<,char-expression…>) | Exists(string) | Exists(string~{ expression }) | FileExists(char-expression) | StringToName(char-expression) | S2N(char-expression) | GetNumber(char-expression <,expression>) | GetValue("string", expression) | DefineNumber(expression, onelab-options)
Such expressions are used in most of Gmsh’s scripting
commands. When ~{expression}
is appended to a string
string, the result is a new string formed by the concatenation of
string, _
(an underscore) and the value of the
expression. This is most useful in loops (see Loops and conditionals), where it permits to define unique strings
automatically. For example,
For i In {1:3} x~{i} = i; EndFor
is the same as
x_1 = 1; x_2 = 2; x_3 = 3;
The brackets []
permit to extract one item from a list
(parentheses can also be used instead of brackets). The #
permits
to get the size of a list. The operators operator-unary-left,
operator-unary-right, operator-binary,
operator-ternary-left and operator-ternary-right are defined
in Operators. For the definition of built-in-functions,
see Built-in functions. The various real-options are
listed in Options. Find
searches for occurrences of the
first expression in the second (both of which can be lists).
StrFind
searches the first char-expression for any
occurrence of the second char-expression. StrCmp
compares
the two strings (returns an integer greater than, equal to, or less than
0, according as the first string is greater than, equal to, or less than
the second string). StrLen
returns the length of the
string. TextAttributes
creates attributes for text
strings. Exists
checks if a variable with the given name exists
(i.e., has been defined previously), and FileExists
checks if the
file with the given name exists. StringToName
creates a name
from the provided string. GetNumber
allows to get the value of a
ONELAB variable (the optional second argument is the default value
returned if the variable does not exist). GetValue
allows to ask
the user for a value interactively (the second argument is the value
returned in non-interactive mode). For example, inserting
GetValue("Value of parameter alpha?", 5.76)
in an input file will
query the user for the value of a certain parameter alpha, assuming the
default value is 5.76. If the option General.NoPopup
is set
(see General options list), no question is asked and the default
value is automatically used.
DefineNumber
allows to define a ONELAB variable in-line. The
expression given as the first argument is the default value; this
is followed by the various ONELAB options. See the
ONELAB tutorial wiki for more information.
List of expressions are also widely used, and are defined as:
expression-list: expression-list-item <, expression-list-item> …
with
expression-list-item: expression | expression : expression | expression : expression : expression | string [ ] | string ( ) | List [ string ] | List [ expression-list-item ] | List [ { expression-list } ] | Unique [ expression-list-item ] | Abs [ expression-list-item ] | ListFromFile [ expression-char ] | LinSpace[ expression, expression, expression ] | LogSpace[ expression, expression, expression ] | string [ { expression-list } ] | Point { expression } | transform | extrude | boolean | Point|Curve|Surface|Volume In BoundingBox { expression-list } | BoundingBox Point|Curve|Surface|Volume { expression-list } | Mass Curve|Surface|Volume { expression } | CenterOfMass Curve|Surface|Volume { expression } | MatrixOfInertia Curve|Surface|Volume { expression } | Point { expression } | Physical Point|Curve|Surface|Volume { expression-list } | <Physical> Point|Curve|Surface|Volume { : } |
The second case in this last definition permits to create a list
containing the range of numbers comprised between two
expressions, with a unit incrementation step. The third case
also permits to create a list containing the range of numbers comprised
between two expressions, but with a positive or negative
incrementation step equal to the third expression. The fourth,
fifth and sixth cases permit to reference an expression list
(parentheses can also be used instead of brackets). Unique
sorts
the entries in the list and removes all duplicates. Abs
takes
the absolute value of all entries in the list. ListFromFile
reads
a list of numbers from a file. LinSpace
and LogSpace
construct lists using linear or logarithmic spacing. The next two cases
permit to reference an expression sublist (whose elements are those
corresponding to the indices provided by the expression-list).
The next cases permit to retrieve the indices of entities created
through geometrical transformations, extrusions and boolean operations
(see Transformations, Extrusions and Boolean operations).
The next two cases allow to retrieve entities in a given bounding box,
or get the bounding box of a given entity, with the bounding box
specified as (X min, Y min, Z min, X max, Y max, Z max). Beware that the
order of coordinates is different than in the BoundingBox
command
for the scene: see General commands. The last cases permit to
retrieve the mass, the center of mass or the matrix of intertia of an
entity, the coordinates of a given geometry point (see Points), the
elementary entities making up physical groups, and the tags of all
(physical or elementary) points, curves, surfaces or volumes in the
model. These operations all trigger a synchronization of the CAD model with the internal Gmsh model.
To see the practical use of such expressions, have a look at the first
couple of examples in Tutorial. Note that, in order to lighten the
syntax, you can omit the braces {}
enclosing an
expression-list if this expression-list only contains a
single item. Also note that a braced expression-list can be
preceded by a minus sign in order to change the sign of all the
expression-list-items.
For some commands it makes sense to specify all the possible expressions in a list. This is achieved with expression-list-or-all, defined as:
expression-list-or-all: expression-list | :
The meaning of “all” (:
) depends on context. For example,
Curve { : }
will get the ids of all the existing curves in the
model, while Surface { : }
will get the ids of all existing
surfaces.
Next: Color expressions, Previous: Floating point expressions, Up: Expressions [Contents][Index]
Character expressions are defined as:
char-expression: "string" | string | string[ expression ] | Today | OnelabAction | GmshExecutableName | CurrentDirectory | CurrentDir | CurrentFileName StrPrefix ( char-expression ) | StrRelative ( char-expression ) | StrCat ( char-expression <,…> ) | Str ( char-expression <,…> ) | StrChoice ( expression, char-expression, char-expression ) | StrSub( char-expression, expression, expression ) | StrSub( char-expression, expression ) | UpperCase ( char-expression ) | AbsolutePath ( char-expression ) | DirName ( char-expression ) | Sprintf ( char-expression , expression-list ) | Sprintf ( char-expression ) | Sprintf ( char-option ) | GetEnv ( char-expression ) | GetString ( char-expression <,char-expression>) | GetStringValue ( char-expression , char-expression ) | StrReplace ( char-expression , char-expression , char-expression ) NameToString ( string ) | N2S ( string ) | <Physical> Point|Curve|Surface|Volume { expression } | DefineString(char-expression, onelab-options)
Today
returns the current date. OnelabAction
returns the
current ONELAB action (e.g. check
or
compute
). GmshExecutableName
returns the full path of the
Gmsh executable. CurrentDirectory
(or CurrentDir
) and
CurrentFileName
return the directory and file name of the script
being parsed. StrPrefix
and StrRelative
take the prefix
(e.g. to remove the extension) or the relative path of a given file
name. StrCat
and Str
concatenate character expressions
(Str
adds a newline character after each string except the last).
StrChoice
returns the first or second char-expression
depending on the value of expression. StrSub
returns the
portion of the string that starts at the character position given by the
first expression and spans the number of characters given by the
second expression or until the end of the string (whichever comes
first; or always if the second expression is not
provided). UpperCase
converts the char-expression to upper
case. AbsolutePath
returns the absolute path of a
file. DirName
returns the directory of a file. Sprintf
is
equivalent to the sprintf
C function (where char-expression
is a format string that can contain floating point formatting
characters: %e
, %g
, etc.) The various
char-options are listed in Options. GetEnvThe
gets the value of an environment variable from the operating
system. GetString
allows to get a ONELAB string value (the second
optional argument is the default value returned if the variable does not
exist). GetStringValue
asks the user for a value interactively
(the second argument is the value used in non-interactive
mode). StrReplace
’s arguments are: input string, old substring,
new substring (brackets can be used instead of parentheses in Str
and Sprintf
). Physical Point
, etc., or Point
, etc.,
retrieve the name of the physical or elementary entity, if any.
NameToString
converts a variable name into a string.
DefineString
allows to define a ONELAB variable in-line. The
char-expression given as the first argument is the default value;
this is followed by the various ONELAB options. See the
ONELAB tutorial wiki for more information.
Character expressions are mostly used to specify non-numeric options and
input/output file names. See t8
: Post-processing and animations, for an interesting usage of
char-expressions in an animation script.
List of character expressions are defined as:
char-expression-list: char-expression <,…>
Previous: Character expressions, Up: Expressions [Contents][Index]
Colors expressions are hybrids between fixed-length braced expression-lists and strings:
color-expression: char-expression | { expression, expression, expression } | { expression, expression, expression, expression } | color-option
The first case permits to use the X Windows names to refer to colors,
e.g., Red
, SpringGreen
, LavenderBlush3
, …
(see
Common/Colors.h
in the source code for a complete list). The second case permits to
define colors by using three expressions to specify their red, green and
blue components (with values comprised between 0 and 255). The third
case permits to define colors by using their red, green and blue color
components as well as their alpha channel. The last case permits to use
the value of a color-option as a color-expression. The
various color-options are listed in Options.
See t3
: Extruded meshes, ONELAB parameters, options, for an example of the use of color expressions.
Next: Built-in functions, Previous: Expressions, Up: General tools [Contents][Index]
Gmsh’s operators are similar to the corresponding operators in C and C++. Here is the list of the unary, binary and ternary operators currently implemented.
operator-unary-left:
operator-unary-right:
operator-binary:
^
¶Exponentiation.
*
¶Multiplication.
/
¶Division.
%
¶Modulo.
+
¶Addition.
-
¶Subtraction.
==
¶Equality.
!=
¶Inequality.
>
¶Greater.
>=
¶Greater or equality.
<
¶Less.
<=
¶Less or equality.
&&
¶Logical ‘and’.
||
¶Logical ‘or’. (Warning: the logical ‘or’ always implies the evaluation of
both arguments. That is, unlike in C or C++, the second operand of
||
is evaluated even if the first one is true).
operator-ternary-left:
?
¶operator-ternary-right:
:
¶The only ternary operator, formed by operator-ternary-left and operator-ternary-right, returns the value of its second argument if the first argument is non-zero; otherwise it returns the value of its third argument.
The evaluation priorities are summarized below3 (from stronger to
weaker, i.e., *
has a highest evaluation priority than +
).
Parentheses ()
may be used anywhere to change the order of
evaluation:
()
, []
, .
, #
^
!
, ++
, --
, -
(unary)
*
, /
, %
+
, -
<
, >
, <=
, >=
==
, !=
&&
||
?:
=
, +=
, -=
, *=
, /=
Next: User-defined macros, Previous: Operators, Up: General tools [Contents][Index]
A built-in function is composed of an identifier followed by a pair of parentheses containing an expression-list, the list of its arguments. This list of arguments can also be provided in between brackets, instead of parentheses. Here is the list of the built-in functions currently implemented:
build-in-function:
Acos ( expression )
¶Arc cosine (inverse cosine) of an expression in [-1,1]. Returns a value in [0,Pi].
Asin ( expression )
¶Arc sine (inverse sine) of an expression in [-1,1]. Returns a value in [-Pi/2,Pi/2].
Atan ( expression )
¶Arc tangent (inverse tangent) of expression. Returns a value in [-Pi/2,Pi/2].
Atan2 ( expression, expression )
¶Arc tangent (inverse tangent) of the first expression divided by the second. Returns a value in [-Pi,Pi].
Ceil ( expression )
¶Rounds expression up to the nearest integer.
Cos ( expression )
¶Cosine of expression.
Cosh ( expression )
¶Hyperbolic cosine of expression.
Exp ( expression )
¶Returns the value of e (the base of natural logarithms) raised to the power of expression.
Fabs ( expression )
¶Absolute value of expression.
Fmod ( expression, expression )
¶Remainder of the division of the first expression by the second, with the sign of the first.
Floor ( expression )
¶Rounds expression down to the nearest integer.
Hypot ( expression, expression )
¶Returns the square root of the sum of the square of its two arguments.
Log ( expression )
¶Natural logarithm of expression (expression > 0).
Log10 ( expression )
¶Base 10 logarithm of expression (expression > 0).
Max ( expression, expression )
¶Maximum of the two arguments.
Min ( expression, expression )
¶Minimum of the two arguments.
Modulo ( expression, expression )
¶see Fmod( expression, expression )
.
Rand ( expression )
¶Random number between zero and expression.
Round ( expression )
¶Rounds expression to the nearest integer.
Sqrt ( expression )
¶Square root of expression (expression >= 0).
Sin ( expression )
¶Sine of expression.
Sinh ( expression )
¶Hyperbolic sine of expression.
Tan ( expression )
¶Tangent of expression.
Tanh ( expression )
¶Hyperbolic tangent of expression.
Next: Loops and conditionals, Previous: Built-in functions, Up: General tools [Contents][Index]
User-defined macros take no arguments, and are evaluated as if a file
containing the macro body was included at the location of the Call
statement.
Macro string | char-expression
¶Begins the declaration of a user-defined macro named string. The
body of the macro starts on the line after ‘Macro string
’,
and can contain any Gmsh command. A synonym for Macro
is
Function
.
Return
¶Ends the body of the current user-defined macro. Macro declarations cannot be imbricated.
Call string | char-expression ;
¶Executes the body of a (previously defined) macro named string.
See t5
: Mesh sizes, macros, loops, holes in volumes, for an example of a user-defined macro. A
shortcoming of Gmsh’s scripting language is that all variables are
“public”. Variables defined inside the body of a macro will thus be
available outside, too!
Next: General commands, Previous: User-defined macros, Up: General tools [Contents][Index]
Loops and conditionals are defined as follows, and can be imbricated:
For ( expression : expression )
¶Iterates from the value of the first expression to the value of the
second expression, with a unit incrementation step. At each iteration,
the commands comprised between ‘For ( expression :
expression )
’ and the matching EndFor
are executed.
For ( expression : expression : expression )
¶Iterates from the value of the first expression to the value of the
second expression, with a positive or negative incrementation step
equal to the third expression. At each iteration, the commands
comprised between ‘For ( expression : expression :
expression )
’ and the matching EndFor
are executed.
For string In { expression : expression }
¶Iterates from the value of the first expression to the value of the
second expression, with a unit incrementation step. At each iteration,
the value of the iterate is affected to an expression named string,
and the commands comprised between ‘For string In {
expression : expression }
’ and the matching EndFor
are
executed.
For string In { expression : expression : expression }
¶Iterates from the value of the first expression to the value of the
second expression, with a positive or negative incrementation step
equal to the third expression. At each iteration, the value of the
iterate is affected to an expression named string, and the commands
comprised between ‘For string In { expression :
expression : expression }
’ and the matching EndFor
are
executed.
EndFor
¶Ends a matching For
command.
If ( expression )
¶The body enclosed between ‘If ( expression )
’ and the matching
ElseIf
, Else
or EndIf
, is evaluated if expression
is non-zero.
ElseIf ( expression )
¶The body enclosed between ‘ElseIf ( expression )
’ and the next
matching ElseIf
, Else
or EndIf
, is evaluated if
expression is non-zero and none of the expression of the
previous matching codes If
and ElseIf
were non-zero.
Else
¶The body enclosed between Else
and the matching EndIf
is evaluated
if none of the expression of the previous matching codes
If
and ElseIf
were non-zero.
EndIf
¶Ends a matching If
command.
Next: General options, Previous: Loops and conditionals, Up: General tools [Contents][Index]
The following commands can be used anywhere in a Gmsh script:
string = expression;
¶Creates a new expression identifier string, or affects expression to an existing expression identifier. The following expression identifiers are predefined (hardcoded in Gmsh’s parser):
Pi
¶Returns 3.1415926535897932.
GMSH_MAJOR_VERSION
¶Returns Gmsh’s major version number.
GMSH_MINOR_VERSION
¶Returns Gmsh’s minor version number.
GMSH_PATCH_VERSION
¶Returns Gmsh’s patch version number.
MPI_Size
¶Returns the number of processors on which Gmsh is running. It is always
1, except if you compiled Gmsh with ENABLE_MPI
(see Compiling the source code).
MPI_Rank
¶Returns the rank of the current processor.
Cpu
¶Returns the current CPU time (in seconds).
Memory
¶Returns the current memory usage (in Mb).
TotalMemory
¶Returns the total memory available (in Mb).
newp
¶Returns the next available point tag. As explained in Geometry module, a unique tag must be associated with every geometrical point:
newp
permits to know the highest tag already attributed (plus
one). This is mostly useful when writing user-defined macros
(see User-defined macros) or general geometric primitives, when one
does not know a priori which tags are already attributed, and
which ones are still available.
newl
¶Returns the next available curve tag.
news
¶Returns the next available surface tag.
newv
¶Returns the next available volume tag.
newll
¶Returns the next available curve loop tag.
newsl
¶Returns the next available surface loop tag.
newreg
¶Returns the next available region tag. That is, newreg
returns
the maximum of newp
, newl
, news
, newv
,
newll
, newsl
and all physical group tags4.
string = { };
¶Creates a new expression list identifier string
with an
empty list.
string[] = { expression-list };
¶Creates a new expression list identifier string
with the
list expression-list, or affects expression-list to an
existing expression list identifier. Parentheses are also allowed
instead of square brackets; although not recommended, brackets and
parentheses can also be completely ommitted.
string [ { expression-list } ] = { expression-list };
¶Affects each item in the right hand side expression-list to the elements (indexed by the left hand side expression-list) of an existing expression list identifier. The two expression-lists must contain the same number of items. Parentheses can also be used instead of brackets.
string += expression;
¶Adds and affects expression to an existing expression identifier.
string -= expression;
¶Subtracts and affects expression to an existing expression identifier.
string *= expression;
¶Multiplies and affects expression to an existing expression identifier.
string /= expression;
¶Divides and affects expression to an existing expression identifier.
string += { expression-list };
¶Appends expression-list to an existing expression list or creates a new expression list with expression-list.
string -= { expression-list };
¶Removes the items in expression-list from the existing expression list.
string [ { expression-list } ] += { expression-list };
¶Adds and affects, item per item, the right hand side expression-list to an existing expression list identifier. Parentheses can also be used instead of brackets.
string [ { expression-list } ] -= { expression-list };
¶Subtracts and affects, item per item, the right hand side expression-list to an existing expression list identifier. Parentheses can also be used instead of brackets.
string [ { expression-list } ] *= { expression-list };
¶Multiplies and affects, item per item, the right hand side expression-list to an existing expression list identifier. Parentheses can also be used instead of brackets.
string [ { expression-list } ] /= { expression-list };
¶Divides and affects, item per item, the right hand side expression-list to an existing expression list identifier. Parentheses can also be used instead of brackets.
string = char-expression;
¶Creates a new character expression identifier string
with a
given char-expression.
string[] = Str( char-expression-list ) ;
¶Creates a new character expression list identifier string
with a given char-expression-list. Parentheses can also be used
instead of brackets.
string[] += Str( char-expression-list ) ;
¶Appends a character expression list to an existing list. Parentheses can also be used instead of brackets.
DefineConstant[ string = expression|char-expression <, ...>];
¶Creates a new expression identifier string, with value expression, only if has not been defined before.
DefineConstant[ string = { expression|char-expression, onelab-options } <, ...>];
¶Same as the previous case, except that the variable is also exchanged with the ONELAB database if it has not been defined before. See the ONELAB tutorial wiki for more information.
SetNumber( char-expression , expression );
¶Sets the value a numeric ONELAB variable char-expression.
SetString( char-expression , char-expression );
¶Sets the value a string ONELAB variable char-expression.
real-option = expression;
¶Affects expression to a real option.
char-option = char-expression;
¶Affects char-expression to a character option.
color-option = color-expression;
¶Affects color-expression to a color option.
real-option += expression;
¶Adds and affects expression to a real option.
real-option -= expression;
¶Subtracts and affects expression to a real option.
real-option *= expression;
¶Multiplies and affects expression to a real option.
real-option /= expression;
¶Divides and affects expression to a real option.
Abort;
¶Aborts the current script.
Exit;
¶Exits Gmsh.
CreateDir char-expression;
¶Create the directory char-expression.
Printf ( char-expression <, expression-list> );
¶Prints a character expression in the information window and/or on the
terminal. Printf
is equivalent to the printf
C function:
char-expression is a format string that can contain formatting
characters (%f
, %e
, etc.). Note that all expressions
are evaluated as floating point values in Gmsh (see Expressions), so
that only valid floating point formatting characters make sense in
char-expression. See t5
: Mesh sizes, macros, loops, holes in volumes, for an example of the use of
Printf
.
Printf ( char-expression , expression-list ) > char-expression;
¶Same as Printf
above, but output the expression in a file.
Printf ( char-expression , expression-list ) >> char-expression;
¶Same as Printf
above, but appends the expression at the end of
the file.
Warning|Error ( char-expression <, expression-list> );
¶Same as Printf
, but raises a warning or an error.
Merge char-expression;
¶Merges a file named char-expression. This command is equivalent to the ‘File->Merge’ menu in the GUI. If the path in char-expression is not absolute, char-expression is appended to the path of the current file. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
ShapeFromFile( char-expression );
¶Merges a BREP, STEP or IGES file and returns the tags of the highest-dimensional entities. Only available with the OpenCASCADE geometry kernel.
Draw;
¶Redraws the scene.
SplitCurrentWindowHorizontal expression;
¶Splits the current window horizontally, with the ratio given by expression.
SplitCurrentWindowVertical expression;
¶Splits the current window vertically, with the ratio given by expression.
SetCurrentWindow expression;
¶Sets the current window by speficying its index (starting at 0) in the list of all windows. When new windows are created by splits, new windows are appended at the end of the list.
UnsplitWindow;
¶Restore a single window.
SetChanged;
¶Force the mesh and post-processing vertex arrays to be regenerated. Useful e.g. for creating animations with changing clipping planes, etc.
BoundingBox;
¶Recomputes the bounding box of the scene (which is normally computed only after new model entities are added or after files are included or merged). The bounding box is computed as follows:
This operation triggers a synchronization of the CAD model with the internal Gmsh model.
BoundingBox { expression, expression, expression, expression, expression, expression };
¶Forces the bounding box of the scene to the given expressions
(X min, X max, Y min, Y max, Z min, Z max). Beware that order of the
coordinates is different than in the BoundingBox
commands for
model entities: see Floating point expressions.
Delete Model;
¶Deletes the current model (all model entities and their associated meshes).
Delete Physicals;
¶Deletes all physical groups.
Delete Variables;
¶Deletes all the expressions.
Delete Options;
¶Deletes the current options and revert to the default values.
Delete string;
¶Deletes the expression string.
Print char-expression;
¶Prints the graphic window in a file named char-expression, using
the current Print.Format
(see General options list). If the
path in char-expression is not absolute, char-expression is
appended to the path of the current file. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Sleep expression;
¶Suspends the execution of Gmsh during expression seconds.
SystemCall char-expression;
¶Executes a (blocking) system call.
NonBlockingSystemCall char-expression;
¶Executes a (non-blocking) system call.
OnelabRun ( char-expression <, char-expression > )
¶Runs a ONELAB client (first argument is the client name, second optional arguement is the command line).
SetName char-expression;
¶Changes the name of the current model.
SetFactory(char-expression);
¶Changes the current geometry kernel (i.e. determines the CAD kernel that
is used for all subsequent geometrical commands). Currently available
kernels: "Built-in"
and "OpenCASCADE"
.
SyncModel;
¶Forces an immediate transfer from the old geometrical database into the new one (this transfer normally occurs right after a file is read).
NewModel;
¶Creates a new current model.
Include char-expression;
¶Includes the file named char-expression at the current position in the input file. The include command should be given on a line of its own. If the path in char-expression is not absolute, char-expression is appended to the path of the current file.
Previous: General commands, Up: General tools [Contents][Index]
The list of all the general char-options, real-options and color-options (in that order—check the default values to see the actual types) is given in General options list. Most of these options are accessible in the GUI, but not all of them. When running Gmsh interactively, changing an option in the script file will modify the option in the GUI in real time. This permits for example to resize the graphical window in a script, or to interact with animations in the script and in the GUI at the same time.
Next: Mesh module, Previous: General tools, Up: Gmsh [Contents][Index]
Geometries can be constructed in Gmsh using different underlying CAD
kernels. Selecting the CAD kernel in .geo
files is done with the
SetFactory
command. In the Gmsh API, the kernel appears
explicitly in all the relevant functions from the gmsh/model
namespace, with geo
or occ
prefixes for the built-in and
OpenCASCADE kernel, respectively.
The built-in CAD kernel (SetFactory("Built-in")
) provides a
simple CAD engine based on a bottom-up boundary representation approach:
you need to first define points (using the Point
command: see
below), then curves (using Line
, Circle
, Spline
,
…, commands or by extruding points), then surfaces (using for
example the Plane Surface
or Surface
commands, or by
extruding curves), and finally volumes (using the Volume
command
or by extruding surfaces). The OpenCASCADE kernel
(SetFactory("OpenCASCADE")
) allows to build models in the same
bottom-up manner, or by using a constructive solid geometry approach
where solids are defined first. Boolean operations can then be performed
to modify them.
These geometrical model entities are also referred to as “elementary entities” in Gmsh, and are assigned tags (stricly positive global identification numbers) when they are created:
Elementary entities can then be manipulated in various
ways, for example using the Translate
, Rotate
,
Scale
or Symmetry
commands. They can be deleted with the
Delete
command, provided that no higher-dimension entity
references them. Zero or negative tags are reserved by the system for
special uses: do not use them in your scripts.
Groups of elementary entities can also be defined and are called “physical” groups. These physical groups cannot be modified by geometry commands: their only purpose is to assemble elementary entities into larger groups so that they can be referred to later as single entities. As is the case with elementary entities, each physical point, physical curve, physical surface or physical volume must be assigned a unique tag. See Mesh module, for more information about how physical groups affect the way meshes are saved.
Next: Geometry options, Previous: Geometry module, Up: Geometry module [Contents][Index]
The next subsections describe all the available geometry commands in the
scripting language. For the equivalent commands in the Gmsh API, see the
gmsh/model/geo
and gmsh/model/occ
namespaces in Gmsh API.
Note that the following general syntax rule is followed for the definition of model entities: “If an expression defines a new entity, it is enclosed between parentheses. If an expression refers to a previously defined entity, it is enclosed between braces.”
Next: Curves, Previous: Geometry commands, Up: Geometry commands [Contents][Index]
Point ( expression ) = { expression, expression, expression <, expression > };
¶Creates a point. The expression inside the parentheses is the point’s tag; the three first expressions inside the braces on the right hand side give the three X, Y and Z coordinates of the point in the three-dimensional Euclidean space; the optional last expression sets the prescribed mesh element size at that point. See Specifying mesh element sizes, for more information about how this value is used in the meshing process.
Physical Point ( expression | char-expression <, expression> ) <+|->= { expression-list };
¶Creates a physical point. The expression inside the parentheses is the physical point’s tag; the expression-list on the right hand side should contain the tags of all the elementary points that need to be grouped inside the physical point. If a char-expression is given instead instead of expression inside the parentheses, a string label is associated with the physical tag, which can be either provided explicitly (after the comma) or not (in which case a unique tag is automatically created).
Next: Surfaces, Previous: Points, Up: Geometry commands [Contents][Index]
Line ( expression ) = { expression, expression };
¶Creates a straight line segment. The expression inside the parentheses is the line segment’s tag; the two expressions inside the braces on the right hand side give tags of the start and end points of the segment.
Bezier ( expression ) = { expression-list };
¶Creates a Bezier curve. The expression-list contains the tags of the control points.
BSpline ( expression ) = { expression-list };
¶Creates a cubic BSpline. The expression-list contains the tags of the control points. Creates a periodic curve if the first and last points are identical.
Spline ( expression ) = { expression-list };
¶Creates a spline going through the points in expression-list. With the built-in geometry kernel this constructs a Catmull-Rom spline. With the OpenCASCADE kernel, this constructs a C2 BSpline. Creates a periodic curve if the first and last points are identical.
Circle ( expression ) = { expression, expression, expression <, ...> };
¶Creates a circle arc. The three expressions on the right-hand-side define the start point, the center and the end point of the arc. With the built-in geometry kernel the arc should be strictly smaller than Pi. With the OpenCASCADE kernel additional expressions can be provided to define a full circle (4th expression is the radius) or a circle arc between two angles (next 2 expressions).
Ellipse ( expression ) = { expression, expression, expression, <, ...> };
¶Creates an ellipse arc. If four expressions are provided on the right-hand-side they define the start point, the center point, a point anywhere on the major axis and the end point. If the first point is a major axis point, the third expression can be ommitted. With the OpenCASCADE kernel, if between 5 and 7 expressions are provided, the first three define the coordinates of the center, the next two define the major (along the x-axis) and minor radii (along the y-axis), and the next two the start and end angle. Note that OpenCASCADE does not allow creating ellipse arcs with the major radius smaller than the minor radius.
Compound Spline | BSpline ( expression ) = { expression-list } Using expression;
¶Creates a spline or a BSpline from control points sampled on the curves
in expression-list. Using
expression specifies the
number of intervals on each curve to compute the sampling
points. Compound splines and BSplines are only available with the
built-in geometry kernel.
Curve Loop ( expression ) = { expression-list };
¶Creates an oriented loop of curves, i.e. a closed wire. The
expression inside the parentheses is the curve loop’s tag; the
expression-list on the right hand side should contain the tags of
all the curves that constitute the curve loop. A curve loop must be a
closed loop, and the curves should be ordered and oriented (using
negative tags to specify reverse orientation). If the orientation is
correct, but the ordering is wrong, Gmsh will actually reorder the list
internally to create a consistent loop. Although Gmsh supports it, it is
not recommended to specify multiple curve loops (or subloops) in a
single Curve Loop
command. (Curve loops are used to create
surfaces: see Surfaces.)
Wire ( expression ) = { expression-list };
¶Creates a path made of curves. Wires are only available with the
OpenCASCADE kernel. They are used to create ThruSections
and
extrusions along paths.
Physical Curve ( expression | char-expression <, expression> ) <+|->= { expression-list };
¶Creates a physical curve. The expression inside the parentheses is the physical curve’s tag; the expression-list on the right hand side should contain the tags of all the elementary curves that need to be grouped inside the physical curve. If a char-expression is given instead instead of expression inside the parentheses, a string label is associated with the physical tag, which can be either provided explicitly (after the comma) or not (in which case a unique tag is automatically created). In some mesh file formats (e.g. MSH2), specifying negative tags in the expression-list will reverse the orientation of the mesh elements belonging to the corresponding elementary curves in the saved mesh file.
Next: Volumes, Previous: Curves, Up: Geometry commands [Contents][Index]
Plane Surface ( expression ) = { expression-list };
¶Creates a plane surface. The expression inside the parentheses is the plane surface’s tag; the expression-list on the right hand side should contain the tags of all the curve loops defining the surface. The first curve loop defines the exterior boundary of the surface; all other curve loops define holes in the surface. A curve loop defining a hole should not have any curves in common with the exterior curve loop (in which case it is not a hole, and the two surfaces should be defined separately). Likewise, a curve loop defining a hole should not have any curves in common with another curve loop defining a hole in the same surface (in which case the two curve loops should be combined).
Surface ( expression ) = { expression-list } < In Sphere { expression } >;
¶Creates a surface filling. With the built-in kernel, the first curve
loop should be composed of either three or four curves. With the
built-in kernel, the optional In Sphere
argument forces the
surface to be a spherical patch (the extra parameter gives the tag of
the center of the sphere).
BSpline Surface ( expression ) = { expression-list };
¶Creates a BSpline surface filling. Only a single curve loop made of 2, 3
or 4 BSpline curves can be provided. BSpline Surface
is only
available with the OpenCASCADE kernel.
Bezier Surface ( expression ) = { expression-list };
¶Creates a Bezier surface filling. Only a single curve loop made of 2, 3
or 4 Bezier curves can be provided. Bezier Surface
is only
available with the OpenCASCADE kernel.
Disk ( expression ) = { expression-list };
¶Creates a disk. When four expressions are provided on the right hand
side (3 coordinates of the center and the radius), the disk is circular.
A fifth expression defines the radius along Y, leading to an ellipse.
Disk
is only available with the OpenCASCADE kernel.
Rectangle ( expression ) = { expression-list };
¶Creates a rectangle. The 3 first expressions define the lower-left
corner; the next 2 define the width and height. If a 6th expression is
provided, it defines a radius to round the rectangle
corners. Rectangle
is only available with the OpenCASCADE kernel.
Surface Loop ( expression ) = { expression-list } < Using Sewing >;
¶Creates a surface loop (a shell). The expression inside the
parentheses is the surface loop’s tag; the expression-list on the
right hand side should contain the tags of all the surfaces that
constitute the surface loop. A surface loop must always represent a
closed shell, and the surfaces should be oriented consistently (using
negative tags to specify reverse orientation). (Surface loops are used
to create volumes: see Volumes.) With the OpenCASCADE kernel, the
optional Using Sewing
argument allows to build a shell made of
surfaces that share geometrically identical (but topologically
different) curves.
Physical Surface ( expression | char-expression <, expression> ) <+|->= { expression-list };
¶Creates a physical surface. The expression inside the parentheses is the physical surface’s tag; the expression-list on the right hand side should contain the tags of all the elementary surfaces that need to be grouped inside the physical surface. If a char-expression is given instead instead of expression inside the parentheses, a string label is associated with the physical tag, which can be either provided explicitly (after the comma) or not (in which case a unique tag is automatically created). In some mesh file formats (e.g. MSH2), specifying negative tags in the expression-list will reverse the orientation of the mesh elements belonging to the corresponding elementary surfaces in the saved mesh file.
Next: Extrusions, Previous: Surfaces, Up: Geometry commands [Contents][Index]
Volume ( expression ) = { expression-list };
¶Creates a volume. The expression inside the parentheses is the volume’s tag; the expression-list on the right hand side should contain the tags of all the surface loops defining the volume. The first surface loop defines the exterior boundary of the volume; all other surface loops define holes in the volume. A surface loop defining a hole should not have any surfaces in common with the exterior surface loop (in which case it is not a hole, and the two volumes should be defined separately). Likewise, a surface loop defining a hole should not have any surfaces in common with another surface loop defining a hole in the same volume (in which case the two surface loops should be combined).
Sphere ( expression ) = { expression-list };
¶Creates a sphere, defined by the 3 coordinates of its center and a
radius. Additional expressions define 3 angle limits. The first two
optional arguments define the polar angle opening (from -Pi/2 to
Pi/2). The optional ‘angle3’ argument defines the azimuthal opening
(from 0 to 2*Pi). Sphere
is only available with the OpenCASCADE
kernel.
Box ( expression ) = { expression-list };
¶Creates a box, defined by the 3 coordinates of a point and the 3
extents. Box
is only available with the OpenCASCADE kernel.
Cylinder ( expression ) = { expression-list };
¶Creates a cylinder, defined by the 3 coordinates of the center of the
first circular face, the 3 components of the vector defining its axis
and its radius. An additional expression defines the angular
opening. Cylinder
is only available with the OpenCASCADE kernel.
Torus ( expression ) = { expression-list };
¶Creates a torus, defined by the 3 coordinates of its center and 2 radii.
An additional expression defines the angular opening. Torus
is
only available with the OpenCASCADE kernel.
Cone ( expression ) = { expression-list };
¶Creates a cone, defined by the 3 coordinates of the center of the first
circular face, the 3 components of the vector defining its axis and the
two radii of the faces (these radii can be zero). An additional
expression defines the angular opening. Cone
is only available
with the OpenCASCADE kernel.
Wedge ( expression ) = { expression-list };
¶Creates a right angular wedge, defined by the 3 coordinates of the
right-angle point and the 3 extends. An additional parameter defines the
top X extent (zero by default). Wedge
is only available with the
OpenCASCADE kernel.
ThruSections ( expression ) = { expression-list };
¶Creates a volume defined through curve loops. ThruSections
is only
available with the OpenCASCADE kernel.
Ruled ThruSections ( expression ) = { expression-list };
¶Same as ThruSections
, but the surfaces created on the boundary
are forced to be ruled. Ruled ThruSections
is only available with
the OpenCASCADE kernel.
Physical Volume ( expression | char-expression <, expression> ) <+|->= { expression-list };
¶Creates a physical volume. The expression inside the parentheses is the physical volume’s tag; the expression-list on the right hand side should contain the tags of all the elementary volumes that need to be grouped inside the physical volume. If a char-expression is given instead instead of expression inside the parentheses, a string label is associated with the physical tag, which can be either provided explicitly (after the comma) or not (in which case a unique tag is automatically created).
Next: Boolean operations, Previous: Volumes, Up: Geometry commands [Contents][Index]
Curves, surfaces and volumes can also be created through extrusion of points, curves and surfaces, respectively. Here is the syntax of the geometrical extrusion commands (go to Structured grids, to see how these commands can be extended in order to also extrude the mesh):
extrude:
Extrude { expression-list } { extrude-list }
¶Extrudes all elementary entities (points, curves or surfaces) in extrude-list using a translation. The expression-list should contain three expressions giving the X, Y and Z components of the translation vector.
Extrude { { expression-list }, { expression-list }, expression } { extrude-list }
¶Extrudes all elementary entities (points, curves or surfaces) in extrude-list using a rotation. The first expression-list should contain three expressions giving the X, Y and Z direction of the rotation axis; the second expression-list should contain three expressions giving the X, Y and Z components of any point on this axis; the last expression should contain the rotation angle (in radians). With the built-in geometry kernel the angle should be strictly smaller than Pi.
Extrude { { expression-list }, { expression-list }, { expression-list }, expression } { extrude-list }
¶Extrudes all elementary entities (points, curves or surfaces) in extrude-list using a translation combined with a rotation (to produce a “twist”). The first expression-list should contain three expressions giving the X, Y and Z components of the translation vector; the second expression-list should contain three expressions giving the X, Y and Z direction of the rotation axis, which should match the direction of the translation; the third expression-list should contain three expressions giving the X, Y and Z components of any point on this axis; the last expression should contain the rotation angle (in radians). With the built-in geometry kernel the angle should be strictly smaller than Pi.
Extrude { extrude-list }
¶Extrudes entities in extrude-list using a translation along their normal. Only available with the built-in geometry kernel.
Extrude { extrude-list } Using Wire { expression-list }
¶Extrudes entities in extrude-list along the give wire. Only available with the OpenCASCADE geometry kernel.
ThruSections { expression-list }
¶Creates surfaces through the given curve loops or
wires. ThruSections
is only available with the OpenCASCADE
kernel.
Ruled ThruSections { expression-list }
¶Creates ruled surfaces through the given curve loops or
wires. Ruled ThruSections
is only available with the OpenCASCADE
kernel.
Fillet { expression-list } { expression-list } { expression-list }
¶Fillets volumes (first list) on some curves (second list), using the
provided radii (third list). The radius list can either contain a single
radius, as many radii as curves, or twice as many as curves (in which
case different radii are provided for the begin and end points of the
curves). Fillet
is only available with the OpenCASCADE kernel.
Chamfer { expression-list } { expression-list } { expression-list } { expression-list }
¶Chamfer volumes (first list) on some curves (second list), using the
provided distance (fourth list) measured on the given surfaces (third
list). The distance list can either contain a single distance, as many
distances as curves, or twice as many as curves (in which case the first
in each pair is measured on the given corresponding
surface). Chamfer
is only available with the OpenCASCADE kernel.
with
extrude-list: <Physical> Point | Curve | Surface { expression-list-or-all }; …
As explained in Floating point expressions, extrude can be used in an expression, in which case it returns a list of tags. By default, the list contains the “top” of the extruded entity at index 0 and the extruded entity at index 1, followed by the “sides” of the extruded entity at indices 2, 3, etc. For example:
Point(1) = {0,0,0}; Point(2) = {1,0,0}; Line(1) = {1, 2}; out[] = Extrude{0,1,0}{ Curve{1}; }; Printf("top curve = %g", out[0]); Printf("surface = %g", out[1]); Printf("side curves = %g and %g", out[2], out[3]);
This behaviour can be changed with the
Geometry.ExtrudeReturnLateralEntities
option (see Geometry options list).
Next: Transformations, Previous: Extrusions, Up: Geometry commands [Contents][Index]
Boolean operations can be applied on curves, surfaces and volumes. All boolean operation act on two lists of elementary entities. The first list represents the object; the second represents the tool. The general syntax for boolean operations is as follows:
boolean:
BooleanIntersection { boolean-list } { boolean-list }
¶Computes the intersection of the object and the tool.
BooleanUnion { boolean-list } { boolean-list }
¶Computes the union of the object and the tool.
BooleanDifference { boolean-list } { boolean-list }
¶Subtract the tool from the object.
BooleanFragments { boolean-list } { boolean-list }
¶Computes all the fragments resulting from the intersection of the entities in the object and in the tool, making all interfaces conformal. When applied to entities of different dimensions, the lower dimensional entities will be automatically embedded in the higher dimensional entities if they are not on their boundary.
with
boolean-list: <Physical> Curve | Surface | Volume { expression-list-or-all }; … | Delete ;
If Delete
is specified in the boolean-list, the tool and/or
the object is deleted.
As explained in Floating point expressions, boolean can be used in an expression, in which case it returns the list of tags of the highest dimensional entities created by the boolean operation. See demos/boolean for examples.
An alternative syntax exists for boolean operations, which can be used when it is known beforehand that the operation will result in a single (highest-dimensional) entity:
boolean-explicit:
BooleanIntersection ( expression ) = { boolean-list } { boolean-list };
¶Computes the intersection of the object and the tool and assign the result the tag expression.
BooleanUnion ( expression ) = { boolean-list } { boolean-list };
¶Computes the union of the object and the tool and assign the result the tag expression.
BooleanDifference ( expression ) = { boolean-list } { boolean-list };
¶Subtract the tool from the object and assign the result the tag expression.
Again, see demos/boolean for examples.
Boolean operations are only available with the OpenCASCADE geometry kernel.
Next: Miscellaneous, Previous: Boolean operations, Up: Geometry commands [Contents][Index]
Geometrical transformations can be applied to elementary entities, or to
copies of elementary entities (using the Duplicata
command: see
below). The syntax of the transformation commands is:
transform:
Dilate { { expression-list }, expression } { transform-list }
¶Scales all elementary entities in transform-list by a factor expression. The expression-list should contain three expressions giving the X, Y, and Z coordinates of the center of the homothetic transformation.
Dilate { { expression-list }, { expression, expression, expression } } { transform-list }
¶Scales all elementary entities in transform-list using different factors along X, Y and Z (the three expressions). The expression-list should contain three expressions giving the X, Y, and Z coordinates of the center of the homothetic transformation.
Rotate { { expression-list }, { expression-list }, expression } { transform-list }
¶Rotates all elementary entities in transform-list by an angle of expression radians. The first expression-list should contain three expressions giving the X, Y and Z direction of the rotation axis; the second expression-list should contain three expressions giving the X, Y and Z components of any point on this axis.
Symmetry { expression-list } { transform-list }
¶Transforms all elementary entities symmetrically to a plane. The expression-list should contain four expressions giving the coefficients of the plane’s equation.
Affine { expression-list } { transform-list }
¶Applies a 4 x 4 affine transformation matrix (16 entries given by row; only 12 can be provided for convenience) to all elementary entities. Currently only available with the OpenCASCADE kernel.
Translate { expression-list } { transform-list }
¶Translates all elementary entities in transform-list. The expression-list should contain three expressions giving the X, Y and Z components of the translation vector.
Boundary { transform-list }
¶(Not a transformation per-se.) Returns the entities on the boundary of
the elementary entities in transform-list, with signs indicating
their orientation in the boundary. To get unsigned tags (e.g. to reuse
the output in other commands), apply the Abs
function on the
returned list. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
CombinedBoundary { transform-list }
¶(Not a transformation per-se.) Returns the boundary of the elementary entities, combined as if a single entity, in transform-list. Useful to compute the boundary of a complex part. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
PointsOf { transform-list }
¶(Not a transformation per-se.) Returns all the geometrical points on the boundary of the elementary entities. Useful to compute the boundary of a complex part. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Intersect Curve { expression-list } Surface { expression }
¶(Not a transformation per-se.) Returns the intersections of the curves given in expression-list with the specified surface. Currently only available with the built-in kernel.
Split Curve { expression } Point { expression-list }
¶(Not a transformation per-se.) Returns the curves created by splitting curve expression on the speficied points. Currently only available with the built-in kernel.
with
transform-list: <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … | Duplicata { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … } | transform
Previous: Transformations, Up: Geometry commands [Contents][Index]
Here is a list of all other geometry commands currently available:
Coherence;
¶Removes all duplicate elementary entities (e.g., points having identical
coordinates). Note that with the built-in geometry kernel Gmsh executes
the Coherence
command automatically after each geometrical
transformation, unless Geometry.AutoCoherence
is set to zero
(see Geometry options list). With the OpenCASCADE geoemtry kernel,
Coherence
is simply a shortcut for a BooleanFragments
operation on all entities.
< Recursive > Delete { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Deletes all elementary entities whose tags are given
in expression-list-or-all. If an entity is linked to another
entity (for example, if a point is used as a control point of a curve),
Delete
has no effect (the curve will have to be deleted before the
point can). The Recursive
variant deletes the entities as well as
all its sub-entities of lower dimension. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Delete Embedded { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Deletes all the embedded entities in the elementary entities whose tags are given in expression-list-or-all. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
SetMaxTag Point | Curve | Surface | Volume ( expression )
¶Forces the maximum tag for a category of entities to a given value, so that subsequently created entities in the same category will not have tags smaller than the given value.
< Recursive > Hide { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Hide the entities listed in expression-list-or-all, if
General.VisibilityMode
is set to 0
or 1
.
Hide { : }
¶Hide all entities, if General.VisibilityMode
is set to 0
or 1
.
< Recursive > Show { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Show the entities listed in expression-list-or-all, if
General.VisibilityMode
is set to 0
or 1
.
Show { : }
¶Show all entities, if General.VisibilityMode
is set to 0
or 1
.
Previous: Geometry commands, Up: Geometry module [Contents][Index]
The list of all the options that control the behavior of geometry commands, as well as the way model entities are handled in the GUI, is given in Geometry options list.
Next: Solver module, Previous: Geometry module, Up: Gmsh [Contents][Index]
Gmsh’s mesh module regroups several 1D, 2D and 3D meshing algorithms, all producing grids conforming in the sense of finite elements (see Mesh: finite element mesh generation):
Recombine
commands (see Structured grids, and
Miscellaneous). The 3D structured algorithms
generate tetrahedra, hexahedra, prisms and pyramids, depending on the
type of the surface meshes they are based on.
All meshes can be subdivided to generate fully quadrangular or fully
hexahedral meshes with the Mesh.SubdivisionAlgorihm
option
(see Mesh options list).
Next: Elementary entities vs. physical groups, Previous: Mesh module, Up: Mesh module [Contents][Index]
Gmsh provides a choice between several 2D and 3D unstructured algorithms. Each algorithm has its own advantages and disadvantages.
For all 2D unstructured algorithms a Delaunay mesh that contains all the points of the 1D mesh is initially constructed using a divide-and-conquer algorithm5. Missing edges are recovered using edge swaps6. After this initial step several algorithms can be applied to generate the final mesh:
For very complex curved surfaces the “MeshAdapt” algorithm is the most robust. When high element quality is important, the “Frontal-Delaunay” algorithm should be tried. For very large meshes of plane surfaces the “Delaunay” algorithm is the fastest; it usually also handles complex mesh size fields better than the “Frontal-Delaunay”. When the “Delaunay” or “Frontal-Delaunay” algorithms fail, “MeshAdapt” is automatically triggered. The “Automatic” algorithm uses “Delaunay” for plane surfaces and “MeshAdapt” for all other surfaces.
Several 3D unstructured algorithms are also available:
The “Delaunay” algorithm is currently the most robust and is the only
one that supports the automatic generation of hybrid meshes with
pyramids. Embedded model entities and the Field
mechanism to
specify element sizes (see Specifying mesh element sizes) are
currently only supported by the “Delaunay” and “HXT” algorithms.
If your version of Gmsh is compiled with OpenMP support (see Compiling the source code), most of the meshing steps can be performed in parallel:
The number of threads can be controlled with the -nt
flag on the
command line (see Command-line options), or with the
General.NumThreads
, Mesh.MaxNumThreads1D
,
Mesh.MaxNumThreads2D
and Mesh.MaxNumThreads3D
options (see
General options list and Mesh options list).
Next: Mesh commands, Previous: Choosing the right unstructured algorithm, Up: Mesh module [Contents][Index]
It is usually convenient to combine elementary geometrical entities into more meaningful groups, e.g. to define some mathematical (“domain”, “boundary with Neumann condition”), functional (“left wing”, “fuselage”) or material (“steel”, “carbon”) properties. Such grouping is done in Gmsh’s geometry module (see Geometry module) through “physical groups”.
By default in the MSH file format and in most other formats (see File formats), if physical groups are defined, the output mesh only contains those elements that belong to at least one physical group. (Different mesh file formats treat physical groups in slightly different ways, depending on their capability to define groups.)
To save all mesh elements wether or not physical groups are defined, use
the Mesh.SaveAll
option (see Mesh options list) or specify
-save_all
on the command line. In some formats (e.g. MSH2),
setting Mesh.SaveAll=1
will however discard all physical group
definitions.
Next: Mesh options, Previous: Elementary entities vs. physical groups, Up: Mesh module [Contents][Index]
The mesh module commands allow to modify the mesh element sizes and specify structured grid parameters. Certain mesh “actions” (i.e., “mesh the curves”, “mesh the surfaces” and “mesh the volumes”) can also be specified in the script files but are usually performed either in the GUI or on the command line (see Running Gmsh on your system, and Command-line options).
In the Gmsh API, the mesh commands are available in the
gmsh/model/mesh
module (see Gmsh API).
Next: Structured grids, Previous: Mesh commands, Up: Mesh commands [Contents][Index]
There are several ways to specify the size of the mesh elements for a given geometry:
Mesh.MeshSizeFromPoints
and
Mesh.MeshSizeExtendFromBoundary
are set (they are by default; see
Mesh options list), you can simply specify desired mesh element
sizes at the geometrical points of the model. The size of the mesh
elements will then be computed by interpolating these values inside the
domain during mesh generation. This might sometimes lead to
over-refinement in some areas, so that you may have to add “dummy”
geometrical entities in the model in order to get the desired element
sizes or use more advanced methods explained below.
Mesh.MeshSizeFromCurvature
is set to a positive value
(it is set to 0 by default), the mesh will be adapted with respect to
the curvature of the model entities, the value giving the target number
of elements per 2 Pi radians.
Box
field specifies the size of the elements inside and
outside of a parallelepipedic region.
Distance
field specifies the size of the mesh according to
the distance to some model entities.
MathEval
field specifies the size of the mesh using an
explicit mathematical function.
PostView
field specifies an explicit background mesh in the
form of a scalar post-processing view (see Post-processing commands, and File formats) in which the nodal values are the
target element sizes. This method is very general but it requires a
first (usually rough) mesh and a way to compute the target sizes on this
mesh (usually through an error estimation procedure, in an iterative
process of mesh adaptation). Warning: only parsed (.pos) files
can currently be used as background meshes (.msh files cannot be
used, since the mesh used to define the field will be destroyed during
the meshing process). (Note that you can also load a background mesh
directly from the command line using the -bgm
option
(see Command-line options), or in the GUI by selecting ‘Apply as
background mesh’ in the post-processing view option menu.)
Min
field specifies the size as the minimum of the sizes
computed using other fields.
The list of available fields with their options is given below. An
example is available in t10
: Mesh size fields.
gmsh/model/mesh/setSizeCallback
(see Namespace gmsh/model/mesh
: mesh functions).
All the aforementioned methods can be used simultaneously, in which case
the smallest element size is selected at any given point. In addition,
boundary mesh sizes (on curves or surfaces) are interpolated inside the
enclosed entity (surface or volume, respectively) if the option
Mesh.MeshSizeExtendFromBoundary
is set (it is by default).
All element sizes are further constrained in the interval [
Mesh.MeshSizeMin
, Mesh.MeshSizeMax
] (which can also be
provided on the command line with -clmin
and -clmax
). The
resulting value is then finally multiplied by Mesh.MeshSizeFactor
(-clscale
on the command line).
Note that when the element size is fully specified by a background mesh field, it is thus often desirable to set
Mesh.MeshSizeFromPoints = 0; Mesh.MeshSizeFromCurvature = 0; Mesh.MeshSizeExtendFromBoundary = 0;
to prevent over-refinement inside an entity due to small mesh sizes on its boundary.
Here are the mesh commands that are related to the specification of mesh element sizes:
MeshSize { expression-list } = expression;
¶Modify the prescribed mesh element size of the points whose tags are listed in expression-list. The new value is given by expression.
Field[expression] = string;
¶Create a new field (with tag expression), of type string.
Field[expression].string = char-expression | expression | expression-list;
¶Set the option string of the expression-th field.
Background Field = expression;
¶Select the expression-th field as the one used to compute element
sizes. Only one background field can be given; if you want to combine
several field, use the Min
or Max
field (see below).
Here is the list of all available fields with their associated options:
Attractor
¶Compute the distance to the given points, curves or surfaces. (Curves are replaced by NumPointsPerCurve equidistant points, to which the distance is actually computed. In the same way, surfaces are replaced by a point cloud, sampled according to NumPointsPerCurve and the size of their bounding box). The Attractor field is deprecated: use the Distance field instead.
Options:
CurvesList
Tags of curves in the geometric model
type: list
default value: {}
FieldX
Tag of the field to use as x coordinate
type: integer
default value: -1
FieldY
Tag of the field to use as y coordinate
type: integer
default value: -1
FieldZ
Tag of the field to use as z coordinate
type: integer
default value: -1
NumPointsPerCurve
Number of points used to discretize each curve (and surface, relative to their bounding box size)
type: integer
default value: 20
PointsList
Tags of points in the geometric model
type: list
default value: {}
SurfacesList
Tags of surfaces in the geometric model
type: list
default value: {}
AttractorAnisoCurve
¶Compute the distance to the given curves and specify the mesh size independently in the direction normal and parallel to the nearest curve. (Each curve is replaced by NumPointsPerCurve equidistant points, to which the distance is actually computed.)
Options:
CurvesList
Tags of curves in the geometric model
type: list
default value: {}
DistMax
Maxmium distance, above this distance from the curves, prescribe the maximum mesh sizes
type: float
default value: 0.5
DistMin
Minimum distance, below this distance from the curves, prescribe the minimum mesh sizes
type: float
default value: 0.1
NumPointsPerCurve
Number of points used to discretized each curve
type: integer
default value: 20
SizeMaxNormal
Maximum mesh size in the direction normal to the closest curve
type: float
default value: 0.5
SizeMaxTangent
Maximum mesh size in the direction tangeant to the closest curve
type: float
default value: 0.5
SizeMinNormal
Minimum mesh size in the direction normal to the closest curve
type: float
default value: 0.05
SizeMinTangent
Minimum mesh size in the direction tangeant to the closest curve
type: float
default value: 0.5
AutomaticMeshSizeField
¶Compute a mesh size field that is quite automatic Takes into account surface curvatures and closeness of objects
Options:
features
Enable computation of local feature size (thin channels)
type: boolean
default value: 1
gradation
Maximum growth ratio for the edges lengths
type: float
default value: 1.1
hBulk
Default size where it is not prescribed
type: float
default value: -1
hMax
Maximum size
type: float
default value: -1
hMin
Minimum size
type: float
default value: -1
nPointsPerCircle
Number of points per circle (adapt to curvature of surfaces)
type: integer
default value: 20
nPointsPerGap
Number of layers of elements in thin layers
type: integer
default value: 0
p4estFileToLoad
p4est file containing the size field
type: string
default value: ""
smoothing
Enable size smoothing (should always be true)
type: boolean
default value: 1
Ball
¶The value of this field is VIn inside a spherical ball, VOut outside. The ball is defined by
||dX||^2 < R^2 &&
dX = (X - XC)^2 + (Y-YC)^2 + (Z-ZC)^2
If Thickness is > 0, the mesh size is interpolated between VIn and VOut in a layer around the ball of the prescribed thickness.
Options:
Radius
Radius
type: float
default value: 0
Thickness
Thickness of a transition layer outside the ball
type: float
default value: 0
VIn
Value inside the ball
type: float
default value: 0
VOut
Value outside the ball
type: float
default value: 0
XCenter
X coordinate of the ball center
type: float
default value: 0
YCenter
Y coordinate of the ball center
type: float
default value: 0
ZCenter
Z coordinate of the ball center
type: float
default value: 0
BoundaryLayer
¶Insert a 2D boundary layer mesh next to some curves in the model.
Options:
AnisoMax
Threshold angle for creating a mesh fan in the boundary layer
type: float
default value: 10000000000
Beta
Beta coefficient of the Beta Law
type: float
default value: 1.01
BetaLaw
Use Beta Law instead of geometric progression
type: integer
default value: 0
CurvesList
Tags of curves in the geometric model for which a boundary layer is needed
type: list
default value: {}
ExcludedSurfacesList
Tags of surfaces in the geometric model where the boundary layer should not be contructed
type: list
default value: {}
FanPointsList
Tags of points in the geometric model for which a fan is created
type: list
default value: {}
FanPointsSizesList
Number of elements in the fan for each fan node. If not present default value Mesh.BoundaryLayerFanElements
type: list
default value: {}
IntersectMetrics
Intersect metrics of all surfaces
type: integer
default value: 0
NbLayers
Number of Layers in theBeta Law
type: integer
default value: 10
PointsList
Tags of points in the geometric model for which a boundary layer ends
type: list
default value: {}
Quads
Generate recombined elements in the boundary layer
type: integer
default value: 0
Ratio
Size ratio between two successive layers
type: float
default value: 1.1
Size
Mesh size normal to the curve
type: float
default value: 0.1
SizeFar
Element size far from the curves
type: float
default value: 1
SizesList
Mesh size normal to the curve, per point (overwrites Size when defined)
type: list_double
default value: {}
Thickness
Maximal thickness of the boundary layer
type: float
default value: 0.01
Box
¶The value of this field is VIn inside the box, VOut outside the box. The box is defined by
Xmin <= x <= XMax &&
YMin <= y <= YMax &&
ZMin <= z <= ZMax
If Thickness is > 0, the mesh size is interpolated between VIn and VOut in a layer around the box of the prescribed thickness.
Options:
Thickness
Thickness of a transition layer outside the box
type: float
default value: 0
VIn
Value inside the box
type: float
default value: 0
VOut
Value outside the box
type: float
default value: 0
XMax
Maximum X coordinate of the box
type: float
default value: 0
XMin
Minimum X coordinate of the box
type: float
default value: 0
YMax
Maximum Y coordinate of the box
type: float
default value: 0
YMin
Minimum Y coordinate of the box
type: float
default value: 0
ZMax
Maximum Z coordinate of the box
type: float
default value: 0
ZMin
Minimum Z coordinate of the box
type: float
default value: 0
Curvature
¶Compute the curvature of Field[InField]:
F = div(norm(grad(Field[InField])))
Options:
Delta
Step of the finite differences
type: float
default value: 0
InField
Input field tag
type: integer
default value: 1
Cylinder
¶The value of this field is VIn inside a frustrated cylinder, VOut outside. The cylinder is given by
||dX||^2 < R^2 &&
(X-X0).A < ||A||^2
dX = (X - X0) - ((X - X0).A)/(||A||^2) . A
Options:
Radius
Radius
type: float
default value: 0
VIn
Value inside the cylinder
type: float
default value: 0
VOut
Value outside the cylinder
type: float
default value: 0
XAxis
X component of the cylinder axis
type: float
default value: 0
XCenter
X coordinate of the cylinder center
type: float
default value: 0
YAxis
Y component of the cylinder axis
type: float
default value: 0
YCenter
Y coordinate of the cylinder center
type: float
default value: 0
ZAxis
Z component of the cylinder axis
type: float
default value: 1
ZCenter
Z coordinate of the cylinder center
type: float
default value: 0
Distance
¶Compute the distance to the given points, curves or surfaces. (Curves are replaced by NumPointsPerCurve equidistant points, to which the distance is actually computed. In the same way, surfaces are replaced by a point cloud, sampled according to NumPointsPerCurve and the size of their bounding box).
Options:
CurvesList
Tags of curves in the geometric model
type: list
default value: {}
FieldX
Id of the field to use as x coordinate
type: integer
default value: -1
FieldY
Id of the field to use as y coordinate
type: integer
default value: -1
FieldZ
Id of the field to use as z coordinate
type: integer
default value: -1
NumPointsPerCurve
Number of points used to discretized each curve (and surface, relative to their bounding box size)
type: integer
default value: 20
PointsList
Tags of points in the geometric model
type: list
default value: {}
SurfacesList
Tags of surfaces in the geometric model
type: list
default value: {}
ExternalProcess
¶**This Field is experimental**
Call an external process that received coordinates triple (x,y,z) as binary double precision numbers on stdin and is supposed to write the field value on stdout as a binary double precision number.
NaN,NaN,NaN is sent as coordinate to indicate the end of the process.
Example of client (python2):
import os
import struct
import math
import sys
if sys.platform == "win32" :
import msvcrt
msvcrt.setmode(0, os.O_BINARY)
msvcrt.setmode(1, os.O_BINARY)
while(True):
____xyz = struct.unpack("ddd", os.read(0,24))
____if math.isnan(xyz[0]):
_________break
____f = 0.001 + xyz[1]*0.009
____os.write(1,struct.pack("d",f))
Example of client (python3):
import struct
import sys
import math
while(True):
____xyz = struct.unpack("ddd", sys.stdin.buffer.read(24))
____if math.isnan(xyz[0]):
________break
____f = 0.001 + xyz[1]*0.009
____sys.stdout.buffer.write(struct.pack("d",f))
____sys.stdout.flush()
Example of client (c, unix):
#include <unistd.h>
int main(int argc, char **argv) {
__double xyz[3];
__while(read(STDIN_FILENO, &xyz, 3*sizeof(double)) == 3*sizeof(double)) {
____if (xyz[0] != xyz[0]) break; //nan
____double f = 0.001 + 0.009 * xyz[1];
____write(STDOUT_FILENO, &f, sizeof(double));
__}
__return 0;
}
Example of client (c, windows):
#include <stdio.h>
#include <io.h>
#include <fcntl.h>
int main(int argc, char **argv) {
__double xyz[3];
__setmode(fileno(stdin),O_BINARY);
__setmode(fileno(stdout),O_BINARY);
__while(read(fileno(stdin), &xyz, 3*sizeof(double)) == 3*sizeof(double)) {
____if (xyz[0] != xyz[0])
______break;
____double f = f = 0.01 + 0.09 * xyz[1];
____write(fileno(stdout), &f, sizeof(double));
__}
}
Options:
CommandLine
Command line to launch
type: string
default value: ""
Frustum
¶This field is an extended cylinder with inner (i) and outer (o) radiuseson both endpoints (1 and 2). Length scale is bilinearly interpolated betweenthese locations (inner and outer radiuses, endpoints 1 and 2)The field values for a point P are given by : u = P1P.P1P2/||P1P2|| r = || P1P - u*P1P2 || Ri = (1-u)*R1i + u*R2i Ro = (1-u)*R1o + u*R2o v = (r-Ri)/(Ro-Ri) lc = (1-v)*( (1-u)*v1i + u*v2i ) + v*( (1-u)*v1o + u*v2o ) where (u,v) in [0,1]x[0,1]
Options:
InnerR1
Inner radius of Frustum at endpoint 1
type: float
default value: 0
InnerR2
Inner radius of Frustum at endpoint 2
type: float
default value: 0
InnerV1
Element size at point 1, inner radius
type: float
default value: 0.1
InnerV2
Element size at point 2, inner radius
type: float
default value: 0.1
OuterR1
Outer radius of Frustum at endpoint 1
type: float
default value: 1
OuterR2
Outer radius of Frustum at endpoint 2
type: float
default value: 1
OuterV1
Element size at point 1, outer radius
type: float
default value: 1
OuterV2
Element size at point 2, outer radius
type: float
default value: 1
X1
X coordinate of endpoint 1
type: float
default value: 0
X2
X coordinate of endpoint 2
type: float
default value: 0
Y1
Y coordinate of endpoint 1
type: float
default value: 0
Y2
Y coordinate of endpoint 2
type: float
default value: 0
Z1
Z coordinate of endpoint 1
type: float
default value: 1
Z2
Z coordinate of endpoint 2
type: float
default value: 0
Gradient
¶Compute the finite difference gradient of Field[InField]:
F = (Field[InField](X + Delta/2) - Field[InField](X - Delta/2)) / Delta
Options:
Delta
Finite difference step
type: float
default value: 0
InField
Input field tag
type: integer
default value: 1
Kind
Component of the gradient to evaluate: 0 for X, 1 for Y, 2 for Z, 3 for the norm
type: integer
default value: 0
IntersectAniso
¶Take the intersection of 2 anisotropic fields according to Alauzet.
Options:
FieldsList
Field indices
type: list
default value: {}
Laplacian
¶Compute finite difference the Laplacian of Field[InField]:
F = G(x+d,y,z) + G(x-d,y,z) +
G(x,y+d,z) + G(x,y-d,z) +
G(x,y,z+d) + G(x,y,z-d) - 6 * G(x,y,z),
where G = Field[InField] and d = Delta
Options:
Delta
Finite difference step
type: float
default value: 0.1
InField
Input field tag
type: integer
default value: 1
LonLat
¶Evaluate Field[InField] in geographic coordinates (longitude, latitude):
F = Field[InField](atan(y/x), asin(z/sqrt(x^2+y^2+z^2))
Options:
FromStereo
If = 1, the mesh is in stereographic coordinates: xi = 2Rx/(R+z), eta = 2Ry/(R+z)
type: integer
default value: 0
InField
Tag of the field to evaluate
type: integer
default value: 1
RadiusStereo
Radius of the sphere of the stereograpic coordinates
type: float
default value: 6371000
MathEval
¶Evaluate a mathematical expression. The expression can contain x, y, z for spatial coordinates, F0, F1, ... for field values, and mathematical functions.
Options:
F
Mathematical function to evaluate.
type: string
default value: "F2 + Sin(z)"
MathEvalAniso
¶Evaluate a metric expression. The expressions can contain x, y, z for spatial coordinates, F0, F1, ... for field values, and mathematical functions.
Options:
M11
Element 11 of the metric tensor
type: string
default value: "F2 + Sin(z)"
M12
Element 12 of the metric tensor
type: string
default value: "F2 + Sin(z)"
M13
Element 13 of the metric tensor
type: string
default value: "F2 + Sin(z)"
M22
Element 22 of the metric tensor
type: string
default value: "F2 + Sin(z)"
M23
Element 23 of the metric tensor
type: string
default value: "F2 + Sin(z)"
M33
Element 33 of the metric tensor
type: string
default value: "F2 + Sin(z)"
Max
¶Take the maximum value of a list of fields.
Options:
FieldsList
Field indices
type: list
default value: {}
MaxEigenHessian
¶Compute the maximum eigenvalue of the Hessian matrix of Field[InField], with the gradients evaluated by finite differences:
F = max(eig(grad(grad(Field[InField]))))
Options:
Delta
Step used for the finite differences
type: float
default value: 0
InField
Input field tag
type: integer
default value: 1
Mean
¶Simple smoother:
F = (G(x+delta,y,z) + G(x-delta,y,z) +
G(x,y+delta,z) + G(x,y-delta,z) +
G(x,y,z+delta) + G(x,y,z-delta) +
G(x,y,z)) / 7,
where G = Field[InField]
Options:
Delta
Distance used to compute the mean value
type: float
default value: 0.0003464101615137755
InField
Input field tag
type: integer
default value: 0
Min
¶Take the minimum value of a list of fields.
Options:
FieldsList
Field indices
type: list
default value: {}
MinAniso
¶Take the intersection of a list of possibly anisotropic fields.
Options:
FieldsList
Field indices
type: list
default value: {}
Octree
¶Pre compute another field on an octree to speed-up evalution
Options:
InField
Id of the field to represent on the octree
type: integer
default value: 0
Param
¶Evaluate Field[InField] in parametric coordinates:
F = Field[InField](FX,FY,FZ)
See the MathEval Field help to get a description of valid FX, FY and FZ expressions.
Options:
FX
X component of parametric function
type: string
default value: ""
FY
Y component of parametric function
type: string
default value: ""
FZ
Z component of parametric function
type: string
default value: ""
InField
Input field tag
type: integer
default value: 1
PostView
¶Evaluate the post processing view IView.
Options:
CropNegativeValues
return LC_MAX instead of a negative value (this option is needed for backward compatibility with the BackgroundMesh option
type: boolean
default value: 1
ViewIndex
Post-processing view index
type: integer
default value: 0
ViewTag
Post-processing view tag
type: integer
default value: -1
Restrict
¶Restrict the application of a field to a given list of geometrical points, curves, surfaces or volumes.
Options:
CurvesList
Curve tags
type: list
default value: {}
InField
Input field tag
type: integer
default value: 1
PointsList
Point tags
type: list
default value: {}
SurfacesList
Surface tags
type: list
default value: {}
VolumesList
Volume tags
type: list
default value: {}
Structured
¶Linearly interpolate between data provided on a 3D rectangular structured grid.
The format of the input file is:
Ox Oy Oz
Dx Dy Dz
nx ny nz
v(0,0,0) v(0,0,1) v(0,0,2) ...
v(0,1,0) v(0,1,1) v(0,1,2) ...
v(0,2,0) v(0,2,1) v(0,2,2) ...
... ... ...
v(1,0,0) ... ...
where O are the coordinates of the first node, D are the distances between nodes in each direction, n are the numbers of nodes in each direction, and v are the values on each node.
Options:
FileName
Name of the input file
type: path
default value: ""
OutsideValue
Value of the field outside the grid (only used if the "SetOutsideValue" option is true).
type: float
default value: 0
SetOutsideValue
True to use the "OutsideValue" option. If False, the last values of the grid are used.
type: boolean
default value: 0
TextFormat
True for ASCII input files, false for binary files (4 bite signed integers for n, double precision floating points for v, D and O)
type: boolean
default value: 0
Threshold
¶F = SizeMin if Field[InField] <= DistMin,
F = SizeMax if Field[InField] >= DistMax,
F = interpolation between SizeMin and SizeMax if DistMin < Field[InField] < DistMax
Options:
DistMax
Distance from entity after which element size will be SizeMax
type: float
default value: 10
DistMin
Distance from entity up to which element size will be SizeMin
type: float
default value: 1
InField
Tag of the field to evaluate
type: integer
default value: 0
Sigmoid
True to interpolate between SizeMin and LcMax using a sigmoid, false to interpolate linearly
type: boolean
default value: 0
SizeMax
Element size outside DistMax
type: float
default value: 1
SizeMin
Element size inside DistMin
type: float
default value: 0.1
StopAtDistMax
True to not impose element size outside DistMax (i.e., F = a very big value if Field[InField] > DistMax)
type: boolean
default value: 0
Next: Miscellaneous, Previous: Specifying mesh element sizes, Up: Mesh commands [Contents][Index]
Extrude { expression-list } { extrude-list layers }
¶Extrudes both the geometry and the mesh using a translation (see Extrusions). The layers option determines how the mesh is extruded and has the following syntax:
layers:
Layers { expression } | Layers { { expression-list }, { expression-list } } | Recombine < expression >; … QuadTriNoNewVerts <RecombLaterals>; | QuadTriAddVerts <RecombLaterals>; ...
In the first Layers
form, expression gives the number of
elements to be created in the (single) layer. In the second form, the
first expression-list defines how many elements should be created
in each extruded layer, and the second expression-list gives the
normalized height of each layer (the list should contain a sequence of
n numbers 0 < h1 < h2 < … < hn <= 1). See
t3
: Extruded meshes, ONELAB parameters, options, for an example.
For curve extrusions, the Recombine
option will recombine triangles
into quadrangles when possible. For surface extrusions, the
Recombine
option will recombine tetrahedra into prisms, hexahedra or
pyramids.
Please note that, starting with Gmsh 2.0, region tags cannot be
specified explicitly anymore in Layers
commands. Instead, as with
all other geometry commands, you must use the automatically created
entity identifier created by the extrusion command. For example, the
following extrusion command will return the tag of the new “top”
surface in num[0]
and the tag of the new volume in num[1]
:
num[] = Extrude {0,0,1} { Surface{1}; Layers{10}; };
QuadTriNoNewVerts
and QuadTriAddVerts
allow to connect
structured, extruded volumes containing quadrangle-faced elements to
structured or unstructured tetrahedral volumes, by subdividing into
triangles any quadrangles on boundary surfaces shared with tetrahedral
volumes. (They have no effect for 1D or 2D extrusions.)
QuadTriNoNewVerts
subdivides any of the region’s quad-faced 3D
elements that touch these boundary triangles into pyramids, prisms, or
tetrahedra as necessary, all wiothout adding new
nodes. QuadTriAddVerts
works in a simular way, but subdivides 3D
elements touching the boundary triangles by adding a new node inside
each element at the node-based centroid. Either method results in a
structured extrusion with an outer layer of subdivided elements that
interface the inner, unmodified elements to the triangle-meshed region
boundaries.
In some rare cases, due to certain lateral boundary conditions, it may
not be possible make a valid element subdivision with
QuadTriNoNewVerts
without adding additional nodes. In this
case, an internal node is created at the node-based centroid of the
element. The element is then divided using that node. When an internal
node is created with QuadTriNoNewVerts
, the user is alerted by
a warning message sent for each instance; however, the mesh will still
be valid and conformal.
Both QuadTriNoNewVerts
and QuadTriAddVerts
can be used
with the optional RecombLaterals
keyword. By default, the QuadTri
algorithms will mesh any free laterals as triangles, if
possible. RecombLaterals
forces any free laterals to remain as
quadrangles, if possible. Lateral surfaces between two QuadTri regions
will always be meshed as quadrangles.
Note that the QuadTri algorithms will handle all potential meshing conflicts along the lateral surfaces of the extrusion. In other words, QuadTri will not subdivide a lateral that must remain as quadrangles, nor will it leave a lateral as quadrangles if it must be divided. The user should therefore feel free to mix different types of neighboring regions with a QuadTri meshed region; the mesh should work. However, be aware that the top surface of the QuadTri extrusion will always be meshed as triangles, unless it is extruded back onto the original source in a toroidal loop (a case which also works with QuadTri).
QuadTriNoNewVerts
and QuadTriAddVerts
may be used
interchangeably, but QuadTriAddVerts
often gives better element
quality.
If the user wishes to interface a structured extrusion to a tetrahedral volume without modifying the original structured mesh, the user may create dedicated interface volumes around the structured geometry and apply a QuadTri algorithm to those volumes only.
Extrude { { expression-list }, { expression-list }, expression } { extrude-list layers }
¶Extrudes both the geometry and the mesh using a rotation (see Extrusions). The layers option is defined as above. With the built-in geometry kernel the angle should be strictly smaller than Pi. With the OpenCASCADE kernel the angle should be strictly smaller than 2 Pi.
Extrude { { expression-list }, { expression-list }, { expression-list }, expression } { extrude-list layers }
¶Extrudes both the geometry and the mesh using a combined translation and rotation (see Extrusions). The layers option is defined as above. With the built-in geometry kernel the angle should be strictly smaller than Pi. With the OpenCASCADE kernel the angle should be strictly smaller than 2 Pi.
Extrude { Surface { expression-list }; layers < Using Index[expr]; > < Using View[expr]; > < ScaleLastLayer; > }
¶Extrudes a “topological” boundary layer from the specified
surfaces. If no view is specified, the mesh of the boundary layer
entities is created using a gouraud-shaded (smoothed) normal field. If a
scalar view is specified, it locally prescribes the thickness of the
layer. If a vector-valued view is specified it locally prescribes both
the extrusion direction and the thickness. Specifying a boundary layer
index allows to extrude several independent boundary layers (with
independent normal smoothing). ScaleLastLayer
scales the height
of the last (top) layer of each normal’s extrusion by the average length
of the edges in all the source elements that contain the source node
(actually, the average of the averages for each element–edges actually
touching the source node are counted twice). This allows the height of
the last layer to vary along with the size of the source elements in
order to achieve better element quality. For example, in a boundary
layer extruded with the Layers definition ’Layers{ {1,4,2}, {0.5,
0.6, 1.6} },’ a source node adjacent to elements with an overall
average edge length of 5.0 will extrude to have a last layer height =
(1.6-0.6) * 5.0 = 5.0. Topological boundary layers are only available
with the built-in kernel. See
sphere_boundary_layer.geo
or
sphere_boundary_layer_from_view.geo
for .geo
file examples, and
aneurysm.py for an API
example.
The advantage of this approach is that it provides a topological
description of the boundary layer, which means that it can be connected
to other geometrical entities. The disadvantage is that the mesh is just
a “simple” extrusion: no fans, no special treatments of reentrant
corners, etc. Another boundary layer algorithm is currently available
through the BoundaryLayer
field (see Specifying mesh element sizes). It only works in 2D however, and is a meshing constraint: it
works directly at the mesh level, without creating geometrical
entities. See
e.g. BL0.geo or
naca12_2d.geo.
Transfinite Curve { expression-list-or-all } = expression < Using Progression | Bump expression >;
¶Selects the curves in expression-list to be meshed with the 1D
transfinite algorithm. The expression on the right hand side gives
the number of nodes that will be created on the curve (this overrides
any other mesh element size prescription—see Specifying mesh element sizes). The optional argument ‘Using Progression
expression
’ instructs the transfinite algorithm to distribute the
nodes following a geometric progression (Progression 2
meaning
for example that each line element in the series will be twice as long
as the preceding one). The optional argument ‘Using Bump
expression
’ instructs the transfinite algorithm to distribute the
nodes with a refinement at both ends of the curve. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Transfinite Surface { expression-list-or-all } < = { expression-list } > < Left | Right | Alternate | AlternateRight | AlternateLeft > ;
¶Selects surfaces to be meshed with the 2D transfinite algorithm. The
expression-list on the right-hand-side should contain the tags of
three or four points on the boundary of the surface that define the
corners of the transfinite interpolation. If no tags are given, the
transfinite algorithm will try to find the corners automatically. The
optional argument specifies the way the triangles are oriented when the
mesh is not recombined. Alternate
is a synonym for
AlternateRight
. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Transfinite Volume { expression-list } < = { expression-list } > ;
¶Selects five- or six-face volumes to be meshed with the 3D transfinite algorithm. The expression-list on the right-hand-side should contain the tags of the six or eight points on the boundary of the volume that define the corners of the transfinite interpolation. If no tags are given, the transfinite algorithm will try to find the corners automatically. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
TransfQuadTri { expression-list } ;
¶Applies the transfinite QuadTri algorithm on the expression-list
list of volumes. A transfinite volume with any combination of
recombined and un-recombined transfinite boundary surfaces is valid when
meshed with TransfQuadTri
. When applied to non-Transfinite
volumes, TransfQuadTri has no effect on those volumes. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Previous: Structured grids, Up: Mesh commands [Contents][Index]
Here is a list of all other mesh commands currently available:
Mesh expression;
¶Generates expression-D mesh. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
RefineMesh;
¶Refines the current mesh by splitting all elements. If
Mesh.SecondOrderLinear
is set, the new nodes are inserted by
linear interpolatinon. Otherwise they are snapped on the actual
geometry. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
OptimizeMesh char-expression;
¶Optimizes the current mesh with the given algorithm (currently
"Gmsh"
for default tetrahedral mesh optimizer, "Netgen"
for Netgen optimizer, "HighOrder"
for direct high-order mesh
optimizer, "HighOrderElastic"
for high-order elastic smoother,
"HighOrderFastCurving"
for fast curving algorithm,
"Laplace2D"
for Laplace smoothing, "Relocate2D"
and
"Relocate3D"
for node relocation).
AdaptMesh { expression-list } { expression-list } { { expression-list < , … > } };
¶Performs adaptive mesh generation. Documentation not yet available.
RelocateMesh Point | Curve | Surface { expression-list-or-all };
¶Relocates the mesh nodes on the given entities using the parametric coordinates stored in the nodes. Useful for creating perturbation of meshes e.g. for sensitivity analyzes. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
RecombineMesh;
¶Recombine the current mesh into quadrangles. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
SetOrder expression;
¶Changes the order of the elements in the current mesh.
PartitionMesh expression;
¶Partitions the mesh into expression, using current partitioning options.
Point | Curve { expression-list } In Surface { expression };
¶Embed the point(s) or curve(s) in the given surface. The surface mesh will conform to the mesh of the point(s) or curves(s). This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Point | Curve | Surface { expression-list } In Volume { expression };
¶Embed the point(s), curve(s) or surface(s) in the given volume. The volume mesh will conform to the mesh of the corresponding point(s), curve(s) or surface(s). This is only supported with the 3D Delaunay algorithm. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Periodic Curve { expression-list } = { expression-list } ;
¶Force the mesh of the curves on the left-hand side to match the mesh of the curves on the right-hand side (masters). If used after meshing, generate the periodic node correspondence information assuming the mesh of the curves on the left-hand side effectively matches the mesh of the curves on the right-hand side. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Periodic Surface expression { expression-list } = expression { expression-list } ;
¶Force the mesh of the surface on the left-hand side (with boundary edges specified between braces) to match the mesh of the master surface on the right-hand side (with boundary edges specified between braces). If used after meshing, generate the periodic node correspondence information assuming the mesh of the surface on the left-hand side effectively matches the mesh of the master surface on the right-hand side (useful for structured and extruded meshes). This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Periodic Curve | Surface { expression-list } = { expression-list } Affine | Translate { expression-list } ;
¶Force mesh of curves or surfaces on the left-hand side to match the mesh
of the curves or surfaces on the right-hand side (masters), using
prescribed geometrical transformations. If used after meshing, generate
the periodic node correspondence information assuming the mesh of the
curves or surfaces on the left-hand side effectively matches the mesh
of the curves or surfaces on the right-hand side (useful for structured
and extruded meshes). Affine
takes a 4 x 4 affine transformation
matrix given by row (only 12 entries can be provided for convenience);
Translate
takes the 3 components of the translation as in
Transformations. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Periodic Curve | Surface { expression-list } = { expression-list } Rotate { expression-list }, { expression-list }, expression } ;
¶Force the mesh of curves or surfaces on the left-hand side to match the mesh of the curves on the right-hand side (masters), using a rotation specified as in Transformations. If used after meshing, generate the periodic node correspondence information assuming the mesh of the curves or surfaces on the left-hand side effectively matches the mesh of the curves or surfaces on the right-hand side (useful for structured and extruded meshes). This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Coherence Mesh;
¶Removes all duplicate mesh nodes.
CreateTopology < { expression , expression } > ;
¶Creates a boundary representation from the mesh of the current model if the model does not have one (e.g. when imported from mesh file formats with no BRep representation of the underlying model). If the first optional argument is set (or not given), make all volumes and surfaces simply connected first; if the second optional argument is set (or not given), clear any built-in CAD kernel entities and export the discrete entities in the built-in CAD kernel.
CreateGeometry < { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … } > ;
¶Creates a geometry for discrete entities (represented solely by a mesh, without an underlying CAD description), i.e. create a parametrization for discrete curves and surfaces, assuming that each can be parametrized with a single map. If no entities are given, create a geometry for all discrete entities.
ClassifySurfaces { expression , expression , expression < , expression > };
¶Classify (“color”) the surface mesh based on an angle threshold (the
first argument, in radians), and create new discrete surfaces, curves
and points accordingly. If the second argument is set, also create
discrete curves on the boundary if the surface is open. If the third
argument is set, create edges and surfaces than can be reparametrized
with CreateGeometry
. The last optional argument sets an angle
threshold to force splitting of the generated curves.
RenumberMeshNodes;
¶Renumbers the node tags in the current mesh in a contiunous sequence.
RenumberMeshElements;
¶Renumbers the elements tags in the current mesh in a contiunous sequence.
< Recursive > Color color-expression { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Sets the mesh color of the entities in expression-list to color-expression. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
< Recursive > Hide { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Hides the mesh of the entities in expression-list, if
General.VisibilityMode
is set to 0
or
2
. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Hide { : }
¶Hide the mesh of all entities, if General.VisibilityMode
is set
to 0
or 2
. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Recombine Surface { expression-list-or-all } < = expression >;
¶Recombines the triangular meshes of the surfaces listed in expression-list into mixed triangular/quadrangular meshes. The optional expression on the right hand side specifies the maximum difference (in degrees) allowed between the largest angle of a quadrangle and a right angle (a value of 0 would only accept quadrangles with right angles; a value of 90 would allow degenerate quadrangles; default value is 45). This operation triggers a synchronization of the CAD model with the internal Gmsh model.
MeshAlgorithm Surface { expression-list } = expression;
¶Forces the meshing algorithm per surface.
MeshSizeFromBoundary Surface { expression-list } = expression;
¶Forces the mesh size to be extended from the boudnary, or not, per surface.
Compound Curve | Surface { expression-list-or-all } ;
¶Treats the given entities as a single entity when meshing, i.e. perform cross-patch meshing of the entities.
ReverseMesh Curve | Surface { expression-list-or-all } ;
¶Reverses the mesh of the given curve(s) or surface(s). This operation triggers a synchronization of the CAD model with the internal Gmsh model.
ReorientMesh Volume { expression-list } ;
¶Reorients the meshes of the bounding surfaces of the given volumes so that the normals point outward to the volumes. Currently only available with the OpenCASCADE kernel, as it relies on the STL triangulation. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Save char-expression;
¶Saves the mesh in a file named char-expression, using the current
Mesh.Format
(see Mesh options list). If the path in
char-expression is not absolute, char-expression is appended
to the path of the current file. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
< Recursive > Show { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
¶Shows the mesh of the entities in expression-list, if
General.VisibilityMode
is set to 0
or
2
. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Show { : };
¶Shows the mesh of all entities, if General.VisibilityMode
is set
to 0
or 2
. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Smoother Surface { expression-list } = expression;
¶Sets number of elliptic smoothing steps for the surfaces listed in expression-list (smoothing only applies to transfinite meshes at the moment). This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Homology ( { expression-list } ) { { expression-list } , { expression-list } };
¶Compute a basis representation for homology spaces after a mesh has been generated. The first expression-list is a list of dimensions whose homology bases are computed; if empty, all bases are computed. The second expression-list is a list physical groups that constitute the computation domain; if empty, the whole mesh is the domain. The third expression-list is a list of physical groups that constitute the relative subdomain of relative homology computation; if empty, absolute homology is computed. Resulting basis representation chains are stored as physical groups in the mesh.
Cohomology ( { expression-list } ) { { expression-list } , { expression-list } };
¶Similar to command Homology
, but computes a basis representation
for cohomology spaces instead.
Previous: Mesh commands, Up: Mesh module [Contents][Index]
The list of all the options that control the behavior of mesh commands, as well as the way meshes are displayed in the GUI, is given in Mesh options list.
Next: Post-processing module, Previous: Mesh module, Up: Gmsh [Contents][Index]
Solvers and other external codes can be driven by Gmsh through the ONELAB interface (see http://www.onelab.info), which allows to have them share parameters and modeling information.
Using the Gmsh API, you can directly embed Gmsh in your C++, C, Python or Julia solver, use ONELAB for interactive parameter definition and modification, and to create post-processing data on the fly. See prepro.py, custom_gui.py and custom_gui.cpp for examples.
If you prefer to keep codes separate, you can also communicate with Gmsh
through a socket by providing the solver name (Solver.Name0
,
Solver.Name1
, etc.) and the path to the executable
(Solver.Executable0
, Solver.Executable1
, etc.). Parameters
can then be exchanged using the ONELAB protocol: see the
utils/solvers directory for
examples. A full-featured solver interfaced in this manner is GetDP
(https://getdp.info), a general finite element solver using mixed
finite elements.
The list of all the solver options is given in Solver options list.
Next: File formats, Previous: Solver module, Up: Gmsh [Contents][Index]
Gmsh’s post-processing module can handle multiple scalar, vector or
tensor datasets along with the geometry and the mesh. The datasets can
be given in several formats: in human-readable “parsed” format (these
are just part of a standard input script, but are usually put in
separate files with a .pos extension), in native MSH files (ASCII
or binary files with .msh extensions: see File formats), or
in standard third-party formats. Datasets can also be directly imported
using the Gmsh API, in the gmsh/view
module (see Gmsh API).
Once loaded into Gmsh, scalar fields can be displayed as iso-curves,
iso-surfaces or color maps, whereas vector fields can be represented
either by three-dimensional arrows or by displacement maps. Tensor
fields can be displayed as Von-Mises effective stresses, min/max
eigenvalues, eigenvectors, ellipses or ellipsoids. (To display other
(combinations of) components, you can use the Force scalar
or
Force vector
options, or use Plugin(MathEval)
: see
Post-processing plugins.)
In Gmsh’s jargon, each dataset, along with the visualization options, is
called a “post-processing view”, or simply a “view”. Each view is
given a name, and can be manipulated either individually (each view has
its own button in the GUI and can be referred to by its index in a
script or in the API) or globally (see the PostProcessing.Link
option in Post-processing options list).
By default, Gmsh treats all post-processing views as three-dimensional plots, i.e., draws the scalar, vector and tensor primitives (points, curves, triangles, tetrahedra, etc.) in 3D space. But Gmsh can also represent each post-processing view containing scalar points as two-dimensional (“X-Y”) plots, either space- or time-oriented:
Although visualization is usually mostly an interactive task, Gmsh
exposes all the post-processing commands and options to the user in its
scripting language and through the API to permit a complete automation
of the post-processing process (see e.g., t8
: Post-processing and animations, and
t9
: Plugins).
The two following sections summarize all available post-processing commands and options. Most options apply to both 2D and 3D plots (colormaps, point/line sizes, interval types, time step selection, etc.), but some are peculiar to 3D (lightning, element selection, etc.) or 2D plots (abscissa labels, etc.). Note that 2D plots can be positioned explicitly inside the graphical window, or be automatically positioned in order to avoid overlaps.
Sample post-processing files in human-readable “parsed” format and in
the native MSH file format are available in the
tutorial
directory of Gmsh’s distribution (.pos and .msh
files). The “parsed” format is defined in the next section (cf. the
View
command); the MSH format is defined in File formats.
Next: Post-processing plugins, Previous: Post-processing module, Up: Post-processing module [Contents][Index]
This section describes the post-processing commands availanble in the
scripting language. For the equivalent commands in the Gmsh API, see the
gmsh/view
module in Gmsh API.
Alias View[expression];
¶Creates an alias of the expression-th post-processing view.
Note that Alias
creates a logical duplicate of the view without
actually duplicating the data in memory. This is very useful when you want
multiple simultaneous renderings of the same large dataset (usually with
different display options), but you cannot afford to store all copies in
memory. If what you really want is multiple physical copies of the data,
just merge the file containing the post-processing view multiple times.
AliasWithOptions View[expression];
¶Creates an alias of the expression-th post-processing view and copies all the options of the expression-th view to the new aliased view.
CopyOptions View[expression, expression];
¶Copy all the options from the first expression-th post-processing view to the second one.
Combine ElementsByViewName;
¶Combines all the post-processing views having the same name into new views. The combination is done “spatially”, i.e., simply by appending the elements at the end of the new views.
Combine ElementsFromAllViews | Combine Views;
¶Combines all the post-processing views into a single new view. The combination is done “spatially”, i.e., simply by appending the elements at the end of the new view.
Combine ElementsFromVisibleViews;
¶Combines all the visible post-processing views into a single new view. The combination is done “spatially”, i.e., simply by appending the elements at the end of the new view.
Combine TimeStepsByViewName | Combine TimeSteps;
¶Combines the data from all the post-processing views having the same name into new multi-time-step views. The combination is done “temporally”, i.e., as if the data in each view corresponds to a different time instant. The combination will fail if the meshes in all the views are not identical.
Combine TimeStepsFromAllViews;
¶Combines the data from all the post-processing views into a new multi-time-step view. The combination is done “temporally”, i.e., as if the data in each view corresponds to a different time instant. The combination will fail if the meshes in all the views are not identical.
Combine TimeStepsFromVisibleViews;
¶Combines the data from all the visible post-processing views into a new multi-time-step view. The combination is done “temporally”, i.e., as if the data in each view corresponds to a different time instant. The combination will fail if the meshes in all the views are not identical.
Delete View[expression];
¶Deletes (removes) the expression-th post-processing view. Note that post-processing view indices start at 0.
Delete Empty Views;
¶Deletes (removes) all the empty post-processing views.
Background Mesh View[expression];
¶Applies the expression-th post-processing view as the current background mesh. Note that post-processing view indices start at 0.
Plugin (string) . Run;
¶Executes the plugin string. The list of default plugins is given in Post-processing plugins.
Plugin (string) . string = expression | char-expression;
¶Sets an option for a given plugin. See Post-processing plugins, for a
list of default plugins and t9
: Plugins, for some examples.
Save View[expression] char-expression;
¶Saves the expression-th post-processing view in a file named char-expression. If the path in char-expression is not absolute, char-expression is appended to the path of the current file.
SendToServer View[expression] char-expression;
¶Sends the expression-th post-processing view to the ONELAB server, with parameter name char-expression.
View "string" { string < ( expression-list ) > { expression-list }; … };
¶Creates a new post-processing view, named "string"
. This
is an easy and quite powerful way to import post-processing data: all
the values are expressions, you can embed datasets directly into
your geometrical descriptions (see, e.g., t4
: Built-in functions, holes in surfaces, annotations, entity colors), the data can be
easily generated “on-the-fly” (there is no header containing a
priori information on the size of the dataset). The syntax is also very
permissive, which makes it ideal for testing purposes.
However this “parsed format” is read by Gmsh’s script parser, which makes it inefficient if there are many elements in the dataset. Also, there is no connectivity information in parsed views and all the elements are independent (all fields can be discontinuous), so a lot of information can be duplicated. For large datasets, you should thus use the mesh-based post-processing file format described in File formats, or use one of the standard formats like MED.
More explicitly, the syntax for a parsed View
is the following
View "string" { type ( list-of-coords ) { list-of-values }; … < TIME { expression-list }; > < INTERPOLATION_SCHEME { val-coef-matrix } { val-exp-matrix } < { geo-coef-matrix } { geo-exp-matrix } > ; > };
where the 47 object types that can be displayed are:
type #list-of-coords #list-of-values -------------------------------------------------------------------- Scalar point SP 3 1 * nb-time-steps Vector point VP 3 3 * nb-time-steps Tensor point TP 3 9 * nb-time-steps Scalar line SL 6 2 * nb-time-steps Vector line VL 6 6 * nb-time-steps Tensor line TL 6 18 * nb-time-steps Scalar triangle ST 9 3 * nb-time-steps Vector triangle VT 9 9 * nb-time-steps Tensor triangle TT 9 27 * nb-time-steps Scalar quadrangle SQ 12 4 * nb-time-steps Vector quadrangle VQ 12 12 * nb-time-steps Tensor quadrangle TQ 12 36 * nb-time-steps Scalar tetrahedron SS 12 4 * nb-time-steps Vector tetrahedron VS 12 12 * nb-time-steps Tensor tetrahedron TS 12 36 * nb-time-steps Scalar hexahedron SH 24 8 * nb-time-steps Vector hexahedron VH 24 24 * nb-time-steps Tensor hexahedron TH 24 72 * nb-time-steps Scalar prism SI 18 6 * nb-time-steps Vector prism VI 18 18 * nb-time-steps Tensor prism TI 18 54 * nb-time-steps Scalar pyramid SY 15 5 * nb-time-steps Vector pyramid VY 15 15 * nb-time-steps Tensor pyramid TY 15 45 * nb-time-steps 2D text T2 3 arbitrary 3D text T3 4 arbitrary
The coordinates are given ‘by node’, i.e.,
(coord1, coord2, coord3)
for a point,
(coord1-node1, coord2-node1, coord3-node1,
coord1-node2, coord2-node2, coord3-node2)
for a line,
(coord1-node1, coord2-node1, coord3-node1,
coord1-node2, coord2-node2, coord3-node2,
coord1-node3, coord2-node3, coord3-node3)
for a triangle,
The ordering of the nodes is given in Node ordering.
The values are given by time step, by node and by component, i.e.:
comp1-node1-time1, comp2-node1-time1, comp3-node1-time1, comp1-node2-time1, comp2-node2-time1, comp3-node2-time1, comp1-node3-time1, comp2-node3-time1, comp3-node3-time1, comp1-node1-time2, comp2-node1-time2, comp3-node1-time2, comp1-node2-time2, comp2-node2-time2, comp3-node2-time2, comp1-node3-time2, comp2-node3-time2, comp3-node3-time2, …
For the 2D text objects, the two first expressions in list-of-coords give the X-Y position of the string in screen coordinates, measured from the top-left corner of the window. If the first (respectively second) expression is negative, the position is measured from the right (respectively bottom) edge of the window. If the value of the first (respectively second) expression is larger than 99999, the string is centered horizontally (respectively vertically). If the third expression is equal to zero, the text is aligned bottom-left and displayed using the default font and size. Otherwise, the third expression is converted into an integer whose eight lower bits give the font size, whose eight next bits select the font (the index corresponds to the position in the font menu in the GUI), and whose eight next bits define the text alignment (0=bottom-left, 1=bottom-center, 2=bottom-right, 3=top-left, 4=top-center, 5=top-right, 6=center-left, 7=center-center, 8=center-right).
For the 3D text objects, the three first expressions in list-of-coords give the XYZ position of the string in model (real world) coordinates. The fourth expression has the same meaning as the third expression in 2D text objects.
For both 2D and 3D text objects, the list-of-values can contain an
arbitrary number of char-expressions. If the
char-expression starts with file://
, the remainder of the
string is interpreted as the name of an image file, and the image is
displayed instead of the string. A format string in the form
@wxh
or @wxh,wx,wy,wz,hx,hy,hz
, where w
and
h
are the width and height (in model coordinates for T3
or
in pixels for T2
) of the image, wx,wy,wz
is the direction
of the bottom edge of the image and hx,hy,hz
is the direction of
the left edge of the image.
The optional TIME
list can contain a list of expressions giving the
value of the time (or any other variable) for which an evolution was saved.
The optional INTERPOLATION_SCHEME
lists can contain the
interpolation matrices used for high-order adaptive visualization.
Let us assume that the approximation of the view’s value over an element is written as a linear combination of d basis functions f[i], i=0, ..., d-1 (the coefficients being stored in list-of-values). Defining f[i] = Sum(j=0, ..., d-1) F[i][j] p[j], with p[j] = u^P[j][0] v^P[j][1] w^P[j][2] (u, v and w being the coordinates in the element’s parameter space), then val-coef-matrix denotes the d x d matrix F and val-exp-matrix denotes the d x 3 matrix P.
In the same way, let us also assume that the coordinates x, y and z of the element are obtained through a geometrical mapping from parameter space as a linear combination of m basis functions g[i], i=0, ..., m-1 (the coefficients being stored in list-of-coords). Defining g[i] = Sum(j=0, ..., m-1) G[i][j] q[j], with q[j] = u^Q[j][0] v^Q[j][1] w^Q[j][2], then geo-coef-matrix denotes the m x m matrix G and geo-exp-matrix denotes the m x 3 matrix Q.
Here are for example the interpolation matrices for a first order quadrangle:
INTERPOLATION_SCHEME { {1/4,-1/4, 1/4,-1/4}, {1/4, 1/4,-1/4,-1/4}, {1/4, 1/4, 1/4, 1/4}, {1/4,-1/4,-1/4, 1/4} } { {0, 0, 0}, {1, 0, 0}, {0, 1, 0}, {1, 1, 0} };
Next: Post-processing options, Previous: Post-processing commands, Up: Post-processing module [Contents][Index]
Post-processing plugins permit to extend the functionality of Gmsh’s post-processing module. The difference between regular post-processing options (see Post-processing options list) and post-processing plugins is that regular post-processing options only change the way the data is displayed, while post-processing plugins either create new post-processing views, or modify the data stored in a view (in a destructive, non-reversible way).
Plugins are available in the GUI by right-clicking on a view button (or
by clicking on the black arrow next to the view button) and then
selecting the ‘Plugin’ submenu. In the API, plugins are available in the
gmsh/plugin
module (see Gmsh API).
Here is the list of the plugins that are shipped by default with Gmsh:
Plugin(AnalyseMeshQuality)
¶Plugin(AnalyseMeshQuality) analyses the quality of the elements of a given dimension in the current model. Depending on the input parameters it computes the minimum of the Jacobian determinant (J), the IGE quality measure (Inverse Gradient Error) and/or the ICN quality measure (Condition Number). Statistics are printed and, if requested, a model-based post-processing view is created for each quality measure. The plugin can optionally hide elements by comparing the measure to a prescribed threshold.
J is faster to compute but gives information only on element validity while the other measures also give information on element quality. The IGE measure is related to the error on the gradient of the finite element solution. It is the scaled Jacobian for quads and hexes and a new measure for triangles and tetrahedra. The ICN measure is related to the condition number of the stiffness matrix. (See the article "Efficient computation of the minimum of shape quality measures on curvilinear finite elements" for details.)
Parameters:
- ‘JacobianDeterminant’: compute J?
- ‘IGEMeasure’: compute IGE?
- ‘ICNMeasure’: compute ICN?
- ‘HidingThreshold’: hide all elements for which min(mu) is strictly greater than (if ‘ThresholdGreater’ == 1) or less than (if ‘ThresholdGreater’ == 0) the threshold, where mu is ICN if ‘ICNMeasure’ == 1, IGE if ‘IGEMeasure’ == 1 or min(J)/max(J) if ‘JacobianDeterminant’ == 1.
- ‘CreateView’: create a model-based view of min(J)/max(J), min(IGE) and/or min(ICN)?
- ‘Recompute’: force recomputation (set to 1 if the mesh has changed).
- ‘DimensionOfElements’: analyse elements of the given dimension if equal to 1, 2 or 3; analyse 2D and 3D elements if equal to 4; or analyse elements of the highest dimension if equal to -1.
Numeric options:
JacobianDeterminant
Default value: 0
IGEMeasure
Default value: 0
ICNMeasure
Default value: 0
HidingThreshold
Default value: 99
ThresholdGreater
Default value: 1
CreateView
Default value: 0
Recompute
Default value: 0
DimensionOfElements
Default value: -1
Plugin(Annotate)
¶Plugin(Annotate) adds the text string ‘Text’, in font ‘Font’ and size ‘FontSize’, in the view ‘View’. The string is aligned according to ‘Align’.
If ‘ThreeD’ is equal to 1, the plugin inserts the string in model coordinates at the position (‘X’,‘Y’,‘Z’). If ‘ThreeD’ is equal to 0, the plugin inserts the string in screen coordinates at the position (‘X’,‘Y’).
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Annotate) is executed in-place for list-based datasets or creates a new list-based view for other datasets.
String options:
Text
Default value: "My Text"
Font
Default value: "Helvetica"
Align
Default value: "Left"
Numeric options:
X
Default value: 50
Y
Default value: 30
Z
Default value: 0
ThreeD
Default value: 0
FontSize
Default value: 14
View
Default value: -1
Plugin(BoundaryAngles)
¶Plugin(BoundaryAngles) computes the (interior) angles between the line elements on the boundary of all surfaces. The angles, computed modulo 2*Pi, are stored in a new post-processing view, one for each surface. The plugin currently only works for planar surfaces.Available options:- Visible (1=True, 0 = False, Default = 1): Visibility of the Views in the GUI - Save (1=True, 0 = False, Default = 0): Save the Views on disk ?- Remove (1=True, 0 = False, Default = 0): Remove the View from the memory after execution?- Filename (Default = ’Angles_Surface’): Root name for the Views (in case of save / Visibility)- Dir (Default = ”): Output directory (possibly nested) String options:
Filename
Default value: "Angles_Surface"
Dir
Default value: ""
Numeric options:
View
Default value: -1
Save
Default value: 0
Visible
Default value: 0
Remove
Default value: 0
Plugin(Bubbles)
¶Plugin(Bubbles) constructs a geometry consisting of ‘bubbles’ inscribed in the Voronoi of an input triangulation. ‘ShrinkFactor’ allows to change the size of the bubbles. The plugin expects a triangulation in the ‘z = 0’ plane to exist in the current model.
Plugin(Bubbles) creates one ‘.geo’ file.
String options:
OutputFile
Default value: "bubbles.geo"
Numeric options:
ShrinkFactor
Default value: 0
Plugin(Crack)
¶Plugin(Crack) creates a crack around the physical group ‘PhysicalGroup’ of dimension ‘Dimension’ (1 or 2), embedded in a mesh of dimension ‘Dimension’ + 1. The plugin duplicates the nodes and the elements on the crack and stores them in a new discrete curve (‘Dimension’ = 1) or surface (‘Dimension’ = 2). The elements touching the crack on the “negative” side are modified to use the newly generated nodes.If ‘OpenBoundaryPhysicalGroup’ is given (> 0), its nodes are duplicated and the crack will be left open on that (part of the) boundary. Otherwise, the lips of the crack are sealed, i.e., its nodes are not duplicated. For 1D cracks, ‘NormalX’, ‘NormalY’ and ‘NormalZ’ provide the reference normal of the surface in which the crack is supposed to be embedded. Numeric options:
Dimension
Default value: 1
PhysicalGroup
Default value: 1
OpenBoundaryPhysicalGroup
Default value: 0
NormalX
Default value: 0
NormalY
Default value: 0
NormalZ
Default value: 1
Plugin(Curl)
¶Plugin(Curl) computes the curl of the field in the view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Curl) creates one new list-based view.
Numeric options:
View
Default value: -1
Plugin(CurvedBndDist)
¶Plugin(CurvedBndDist) ...
Plugin(CutBox)
¶Plugin(CutBox) cuts the view ‘View’ with a rectangular box defined by the 4 points (‘X0’,‘Y0’,‘Z0’) (origin), (‘X1’,‘Y1’,‘Z1’) (axis of U), (‘X2’,‘Y2’,‘Z2’) (axis of V) and (‘X3’,‘Y3’,‘Z3’) (axis of W).
The number of points along U, V, W is set with the options ‘NumPointsU’, ‘NumPointsV’ and ‘NumPointsW’.
If ‘ConnectPoints’ is zero, the plugin creates points; otherwise, the plugin generates hexahedra, quadrangles, lines or points depending on the values of ‘NumPointsU’, ‘NumPointsV’ and ‘NumPointsW’.
If ‘Boundary’ is zero, the plugin interpolates the view inside the box; otherwise the plugin interpolates the view at its boundary.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(CutBox) creates one new list-based view.
Numeric options:
X0
Default value: 0
Y0
Default value: 0
Z0
Default value: 0
X1
Default value: 1
Y1
Default value: 0
Z1
Default value: 0
X2
Default value: 0
Y2
Default value: 1
Z2
Default value: 0
X3
Default value: 0
Y3
Default value: 0
Z3
Default value: 1
NumPointsU
Default value: 20
NumPointsV
Default value: 20
NumPointsW
Default value: 20
ConnectPoints
Default value: 1
Boundary
Default value: 1
View
Default value: -1
Plugin(CutGrid)
¶Plugin(CutGrid) cuts the view ‘View’ with a rectangular grid defined by the 3 points (‘X0’,‘Y0’,‘Z0’) (origin), (‘X1’,‘Y1’,‘Z1’) (axis of U) and (‘X2’,‘Y2’,‘Z2’) (axis of V).
The number of points along U and V is set with the options ‘NumPointsU’ and ‘NumPointsV’.
If ‘ConnectPoints’ is zero, the plugin creates points; otherwise, the plugin generates quadrangles, lines or points depending on the values of ‘NumPointsU’ and ‘NumPointsV’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(CutGrid) creates one new list-based view.
Numeric options:
X0
Default value: 0
Y0
Default value: 0
Z0
Default value: 0
X1
Default value: 1
Y1
Default value: 0
Z1
Default value: 0
X2
Default value: 0
Y2
Default value: 1
Z2
Default value: 0
NumPointsU
Default value: 20
NumPointsV
Default value: 20
ConnectPoints
Default value: 1
View
Default value: -1
Plugin(CutMesh)
¶Plugin(CutMesh) cuts the mesh of the current GModel with the zero value of the levelset defined with the view ’View’.Sub-elements are created in the new model (polygons in 2D and polyhedra in 3D) and border elements are created on the zero-levelset.
If ‘Split’ is nonzero, the plugin splits the meshalong the edges of the cut elements in the positive side.
If ’SaveTri’ is nonzero, the sub-elements are saved as simplices.
Plugin(CutMesh) creates one new GModel.
Numeric options:
View
Default value: -1
Split
Default value: 0
SaveTri
Default value: 0
Plugin(CutParametric)
¶Plugin(CutParametric) cuts the view ‘View’ with the parametric function (‘X’(u,v), ‘Y’(u,v), ‘Z’(u,v)), using ‘NumPointsU’ values of the parameter u in [‘MinU’, ‘MaxU’] and ‘NumPointsV’ values of the parameter v in [‘MinV’, ‘MaxV’].
If ‘ConnectPoints’ is set, the plugin creates surface or line elements; otherwise, the plugin generates points.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(CutParametric) creates one new list-based view.
String options:
X
Default value: "2 * Cos(u) * Sin(v)"
Y
Default value: "4 * Sin(u) * Sin(v)"
Z
Default value: "0.1 + 0.5 * Cos(v)"
Numeric options:
MinU
Default value: 0
MaxU
Default value: 6.2832
NumPointsU
Default value: 180
MinV
Default value: 0
MaxV
Default value: 6.2832
NumPointsV
Default value: 180
ConnectPoints
Default value: 0
View
Default value: -1
Plugin(CutPlane)
¶Plugin(CutPlane) cuts the view ‘View’ with the plane ‘A’*X + ‘B’*Y + ‘C’*Z + ‘D’ = 0.
If ‘ExtractVolume’ is nonzero, the plugin extracts the elements on one side of the plane (depending on the sign of ‘ExtractVolume’).
If ‘View’ < 0, the plugin is run on the current view.
Plugin(CutPlane) creates one new list-based view.
Numeric options:
A
Default value: 1
B
Default value: 0
C
Default value: 0
D
Default value: -0.01
ExtractVolume
Default value: 0
RecurLevel
Default value: 4
TargetError
Default value: 0
View
Default value: -1
Plugin(CutSphere)
¶Plugin(CutSphere) cuts the view ‘View’ with the sphere (X-‘Xc’)^2 + (Y-‘Yc’)^2 + (Z-‘Zc’)^2 = ‘R’^2.
If ‘ExtractVolume’ is nonzero, the plugin extracts the elements inside (if ‘ExtractVolume’ < 0) or outside (if ‘ExtractVolume’ > 0) the sphere.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(CutSphere) creates one new list-based view.
Numeric options:
Xc
Default value: 0
Yc
Default value: 0
Zc
Default value: 0
R
Default value: 0.25
ExtractVolume
Default value: 0
RecurLevel
Default value: 4
TargetError
Default value: 0
View
Default value: -1
Plugin(DiscretizationError)
¶Plugin(DiscretizationError) computes the error between the mesh and the geometry. It does so by supersampling the elements and computing the distance between the supersampled points dans their projection on the geometry. Numeric options:
SuperSamplingNodes
Default value: 10
Plugin(Distance)
¶Plugin(Distance) computes distances to entities in a mesh.
If ‘PhysicalPoint’, ‘PhysicalLine’ and ‘PhysicalSurface’ are 0, the distance is computed to all the boundaries. Otherwise the distance is computed to the given physical group.
If ‘DistanceType’ is 0, the plugin computes the geometrical Euclidean distance using the naive O(N^2) algorithm. If ‘DistanceType’ > 0, the plugin computes an approximate distance by solving a PDE with a diffusion constant equal to ‘DistanceType’ time the maximum size of the bounding box of the mesh as in [Legrand et al. 2006].
Positive ‘MinScale’ and ‘MaxScale’ scale the distance function.
Plugin(Distance) creates one new list-based view.
Numeric options:
PhysicalPoint
Default value: 0
PhysicalLine
Default value: 0
PhysicalSurface
Default value: 0
DistanceType
Default value: 0
MinScale
Default value: 0
MaxScale
Default value: 0
Plugin(Divergence)
¶Plugin(Divergence) computes the divergence of the field in the view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Divergence) creates one new list-based view.
Numeric options:
View
Default value: -1
Plugin(Eigenvalues)
¶Plugin(Eigenvalues) computes the three real eigenvalues of each tensor in the view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Eigenvalues) creates three new list-based scalar views.
Numeric options:
View
Default value: -1
Plugin(Eigenvectors)
¶Plugin(Eigenvectors) computes the three (right) eigenvectors of each tensor in the view ‘View’ and sorts them according to the value of the associated eigenvalues.
If ‘ScaleByEigenvalues’ is set, each eigenvector is scaled by its associated eigenvalue. The plugin gives an error if the eigenvectors are complex.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Eigenvectors) creates three new list-based vector view.
Numeric options:
ScaleByEigenvalues
Default value: 1
View
Default value: -1
Plugin(ExtractEdges)
¶Plugin(ExtractEdges) extracts sharp edges from a triangular mesh.
Plugin(ExtractEdges) creates one new view.
Numeric options:
Angle
Default value: 40
IncludeBoundary
Default value: 1
Plugin(ExtractElements)
¶Plugin(ExtractElements) extracts some elements from the view ‘View’. If ‘MinVal’ != ‘MaxVal’, it extracts the elements whose ‘TimeStep’-th values (averaged by element) are comprised between ‘MinVal’ and ‘MaxVal’. If ‘Visible’ != 0, it extracts visible elements.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(ExtractElements) creates one new list-based view.
Numeric options:
MinVal
Default value: 0
MaxVal
Default value: 0
TimeStep
Default value: 0
Visible
Default value: 1
Dimension
Default value: -1
View
Default value: -1
Plugin(FieldFromAmplitudePhase)
¶Plugin(FieldFromAmplitudePhase) builds a complex field ’u’ from amplitude ’a’ (complex) and phase ’phi’ given in two different ’Views’ u = a * exp(k*phi), with k the wavenumber.
The result is to be interpolated in a sufficiently fine mesh: ’MeshFile’.
Plugin(FieldFromAmplitudePhase) generates one new view.
String options:
MeshFile
Default value: "fine.msh"
Numeric options:
Wavenumber
Default value: 5
AmplitudeView
Default value: 0
PhaseView
Default value: 1
Plugin(GaussPoints)
¶Given an input mesh, Plugin(GaussPoints) creates a list-based view containing the Gauss points for a given polynomial ‘Order’.
If ‘PhysicalGroup’ is nonzero, the plugin only creates points for the elements belonging to the group.
Numeric options:
Order
Default value: 0
Dimension
Default value: 2
PhysicalGroup
Default value: 0
Plugin(Gradient)
¶Plugin(Gradient) computes the gradient of the field in the view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Gradient) creates one new list-based view.
Numeric options:
View
Default value: -1
Plugin(HarmonicToTime)
¶Plugin(HarmonicToTime) takes the values in the time steps ‘RealPart’ and ‘ImaginaryPart’ of the view ‘View’, and creates a new view containing
‘View’[‘RealPart’] * cos(p) +- ‘View’[‘ImaginaryPart’] * sin(p)
with
p = 2*Pi*k/‘NumSteps’, k = 0, ..., ‘NumSteps’-1
and ’NumSteps’ the total number of time steps
over ’NumPeriods’ periods at frequency ’Frequency’ [Hz].
The ’+’ sign is used if ‘TimeSign’>0, the ’-’ sign otherwise.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(HarmonicToTime) creates one new list-based view.
Numeric options:
RealPart
Default value: 0
ImaginaryPart
Default value: 1
NumSteps
Default value: 20
TimeSign
Default value: -1
Frequency
Default value: 1
NumPeriods
Default value: 1
View
Default value: -1
Plugin(HomologyComputation)
¶Plugin(HomologyComputation) computes representative chains of basis elements of (relative) homology and cohomology spaces.
Define physical groups in order to specify the computation domain and the relative subdomain. Otherwise the whole mesh is the domain and the relative subdomain is empty.
Plugin(HomologyComputation) creates new views, one for each basis element. The resulting basis chains of desired dimension together with the mesh are saved to the given file.
String options:
DomainPhysicalGroups
Default value: ""
SubdomainPhysicalGroups
Default value: ""
ReductionImmunePhysicalGroups
Default value: ""
DimensionOfChainsToSave
Default value: "0, 1, 2, 3"
Filename
Default value: "homology.msh"
Numeric options:
ComputeHomology
Default value: 1
ComputeCohomology
Default value: 0
HomologyPhysicalGroupsBegin
Default value: -1
CohomologyPhysicalGroupsBegin
Default value: -1
CreatePostProcessingViews
Default value: 1
ReductionOmit
Default value: 1
ReductionCombine
Default value: 3
PostProcessSimplify
Default value: 1
ReductionHeuristic
Default value: 1
Plugin(HomologyPostProcessing)
¶Plugin(HomologyPostProcessing) operates on representative basis chains of homology and cohomology spaces. Functionality:
1. (co)homology basis transformation:
’TransformationMatrix’: Integer matrix of the transformation.
’PhysicalGroupsOfOperatedChains’: (Co)chains of a (co)homology space basis to be transformed.
Results a new (co)chain basis that is an integer cobination of the given basis.
2. Make basis representations of a homology space and a cohomology space compatible:
’PhysicalGroupsOfOperatedChains’: Chains of a homology space basis.
’PhysicalGroupsOfOperatedChains2’: Cochains of a cohomology space basis.
Results a new basis for the homology space such that the incidence matrix of the new basis and the basis of the cohomology space is the identity matrix.
Options:
’PhysicalGroupsToTraceResults’: Trace the resulting (co)chains to the given physical groups.
’PhysicalGroupsToProjectResults’: Project the resulting (co)chains to the complement of the given physical groups.
’NameForResultChains’: Post-processing view name prefix for the results.
’ApplyBoundaryOperatorToResults’: Apply boundary operator to the resulting chains.
String options:
TransformationMatrix
Default value: "1, 0; 0, 1"
PhysicalGroupsOfOperatedChains
Default value: "1, 2"
PhysicalGroupsOfOperatedChains2
Default value: ""
PhysicalGroupsToTraceResults
Default value: ""
PhysicalGroupsToProjectResults
Default value: ""
NameForResultChains
Default value: "c"
Numeric options:
ApplyBoundaryOperatorToResults
Default value: 0
Plugin(Integrate)
¶Plugin(Integrate) integrates a scalar field over all the elements of the view ‘View’ (if ‘Dimension’ < 0), or over all elements of the prescribed dimension (if ‘Dimension’ > 0). If the field is a vector field, the circulation/flux of the field over line/surface elements is calculated.
If ‘View’ < 0, the plugin is run on the current view.
If ‘OverTime’ = i > -1 , the plugin integrates the scalar view over time (using the trapezoidal rule) instead of over space, starting at step i. If ‘Visible’ = 1, the plugin only integrates over visible entities.
Plugin(Integrate) creates one new list-based view.
Numeric options:
View
Default value: -1
OverTime
Default value: -1
Dimension
Default value: -1
Visible
Default value: 1
Plugin(Invisible)
¶Plugin(Invisible) deletes (if ‘DeleteElements’ is set) or reverses (if ‘ReverseElements’ is set) all the invisible elements in the current model. Numeric options:
DeleteElements
Default value: 1
ReverseElements
Default value: 0
Plugin(Isosurface)
¶Plugin(Isosurface) extracts the isosurface of value ‘Value’ from the view ‘View’, and draws the ‘OtherTimeStep’-th step of the view ‘OtherView’ on this isosurface.
If ‘ExtractVolume’ is nonzero, the plugin extracts the isovolume with values greater (if ‘ExtractVolume’ > 0) or smaller (if ‘ExtractVolume’ < 0) than the isosurface ‘Value’.
If ‘OtherTimeStep’ < 0, the plugin uses, for each time step in ‘View’, the corresponding time step in ‘OtherView’. If ‘OtherView’ < 0, the plugin uses ‘View’ as the value source.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Isosurface) creates as many list-based views as there are time steps in ‘View’.
Numeric options:
Value
Default value: 0
ExtractVolume
Default value: 0
RecurLevel
Default value: 4
TargetError
Default value: 0
View
Default value: -1
OtherTimeStep
Default value: -1
OtherView
Default value: -1
Plugin(Lambda2)
¶Plugin(Lambda2) computes the eigenvalues Lambda(1,2,3) of the tensor (S_ik S_kj + Om_ik Om_kj), where S_ij = 0.5 (ui,j + uj,i) and Om_ij = 0.5 (ui,j - uj,i) are respectively the symmetric and antisymmetric parts of the velocity gradient tensor.
Vortices are well represented by regions where Lambda(2) is negative.
If ‘View’ contains tensor elements, the plugin directly uses the tensors as the values of the velocity gradient tensor; if ‘View’ contains vector elements, the plugin uses them as the velocities from which to derive the velocity gradient tensor.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Lambda2) creates one new list-based view.
Numeric options:
Eigenvalue
Default value: 2
View
Default value: -1
Plugin(LongitudeLatitude)
¶Plugin(LongituteLatitude) projects the view ‘View’ in longitude-latitude.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(LongituteLatitude) is executed in place.
Numeric options:
View
Default value: -1
Plugin(MakeSimplex)
¶Plugin(MakeSimplex) decomposes all non-simplectic elements (quadrangles, prisms, hexahedra, pyramids) in the view ‘View’ into simplices (triangles, tetrahedra).
If ‘View’ < 0, the plugin is run on the current view.
Plugin(MakeSimplex) is executed in-place.
Numeric options:
View
Default value: -1
Plugin(MathEval)
¶Plugin(MathEval) creates a new view using data from the time step ‘TimeStep’ in the view ‘View’.
If only ‘Expression0’ is given (and ‘Expression1’, ..., ‘Expression8’ are all empty), the plugin creates a scalar view. If ‘Expression0’, ‘Expression1’ and/or ‘Expression2’ are given (and ‘Expression3’, ..., ‘Expression8’ are all empty) the plugin creates a vector view. Otherwise the plugin creates a tensor view.
In addition to the usual mathematical functions (Exp, Log, Sqrt, Sin, Cos, Fabs, etc.) and operators (+, -, *, /, ^), all expressions can contain:
- the symbols v0, v1, v2, ..., vn, which represent the n components in ‘View’;
- the symbols w0, w1, w2, ..., wn, which represent the n components of ‘OtherView’, at time step ‘OtherTimeStep’;
- the symbols x, y and z, which represent the three spatial coordinates.
If ‘TimeStep’ < 0, the plugin extracts data from all the time steps in the view.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(MathEval) creates one new view.If ‘PhysicalRegion’ < 0, the plugin is run on all physical regions.
Plugin(MathEval) creates one new list-based view.
String options:
Expression0
Default value: "Sqrt(v0^2+v1^2+v2^2)"
Expression1
Default value: ""
Expression2
Default value: ""
Expression3
Default value: ""
Expression4
Default value: ""
Expression5
Default value: ""
Expression6
Default value: ""
Expression7
Default value: ""
Expression8
Default value: ""
Numeric options:
TimeStep
Default value: -1
View
Default value: -1
OtherTimeStep
Default value: -1
OtherView
Default value: -1
ForceInterpolation
Default value: 0
PhysicalRegion
Default value: -1
Plugin(MeshSizeFieldView)
¶Plugin(MeshSizeFieldView) evaluates the mesh size field ‘MeshSizeField’ on specified ‘Component‘ (0 for scalar) of the post-processing view ‘View’. Numeric options:
MeshSizeField
Default value: 0
View
Default value: -1
Component
Default value: 0
Plugin(MeshSubEntities)
¶Plugin(MeshSubEntities) creates mesh elements for the entities of dimension ‘OutputDimension’ (0 for vertices, 1 for edges, 2 for faces) of the ‘InputPhysicalGroup’ of dimension ‘InputDimension’. The plugin creates new elements belonging to ‘OutputPhysicalGroup’. Numeric options:
InputDimension
Default value: 1
InputPhysicalGroup
Default value: 1
OuputDimension
Default value: 0
OuputPhysicalGroup
Default value: 2000
Plugin(MeshVolume)
¶Plugin(MeshVolume) computes the volume of the mesh.
Only the elements in the physical group ‘PhysicalGroup’ of dimension ‘Dimension’ are taken into account, unless ’PhysicalGroup’ is negative, in which case all the elements of the given ‘Dimension’ are considered. If ‘Dimension‘ is negative, all the elments are considered.
Plugin(MeshVolume) creates one new list-based view.
Numeric options:
PhysicalGroup
Default value: -1
Dimension
Default value: 3
Plugin(MinMax)
¶Plugin(MinMax) computes the min/max of a view.
If ‘View’ < 0, the plugin is run on the current view. If ‘OverTime’ = 1, the plugin calculates the min/max over space and time. If ‘Argument’ = 1, the plugin calculates the min/max and the argmin/argmax. If ‘Visible’ = 1, the plugin is only applied to visible entities.
Plugin(MinMax) creates two new list-based views.
Numeric options:
View
Default value: -1
OverTime
Default value: 0
Argument
Default value: 0
Visible
Default value: 1
Plugin(ModifyComponents)
¶Plugin(ModifyComponents) modifies the components of the ‘TimeStep’-th time step in the view ‘View’, using the expressions provided in ‘Expression0’, ..., ‘Expression8’. If an expression is empty, the corresponding component in the view is not modified.
The expressions can contain:
- the usual mathematical functions (Log, Sqrt, Sin, Cos, Fabs, ...) and operators (+, -, *, /, ^);
- the symbols x, y and z, to retrieve the coordinates of the current node;
- the symbols Time and TimeStep, to retrieve the current time and time step values;
- the symbols v0, v1, v2, ..., v8, to retrieve each component of the field in ‘View’ at the ‘TimeStep’-th time step;
- the symbols w0, w1, w2, ..., w8, to retrieve each component of the field in ‘OtherView’ at the ‘OtherTimeStep’-th time step. If ‘OtherView’ and ‘View’ are based on different spatial grids, or if their data types are different, ‘OtherView’ is interpolated onto ‘View’.
If ‘TimeStep’ < 0, the plugin automatically loops over all the time steps in ‘View’ and evaluates the expressions for each one.
If ‘OtherTimeStep’ < 0, the plugin uses ‘TimeStep’ instead.
If ‘View’ < 0, the plugin is run on the current view.
If ‘OtherView’ < 0, the plugin uses ‘View’ instead.
Plugin(ModifyComponents) is executed in-place.
String options:
Expression0
Default value: "v0 * Sin(x)"
Expression1
Default value: ""
Expression2
Default value: ""
Expression3
Default value: ""
Expression4
Default value: ""
Expression5
Default value: ""
Expression6
Default value: ""
Expression7
Default value: ""
Expression8
Default value: ""
Numeric options:
TimeStep
Default value: -1
View
Default value: -1
OtherTimeStep
Default value: -1
OtherView
Default value: -1
ForceInterpolation
Default value: 0
Plugin(ModulusPhase)
¶Plugin(ModulusPhase) interprets the time steps ‘realPart’ and ‘imaginaryPart’ in the view ‘View’ as the real and imaginary parts of a complex field and replaces them with their corresponding modulus and phase.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(ModulusPhase) is executed in-place.
Numeric options:
RealPart
Default value: 0
ImaginaryPart
Default value: 1
View
Default value: -1
Plugin(NearToFarField)
¶Plugin(NearToFarField) computes the far field pattern from the near electric E and magnetic H fields on a surface enclosing the radiating device (antenna).
Parameters: the wavenumber, the angular discretisation (phi in [0, 2*Pi] and theta in [0, Pi]) of the far field sphere and the indices of the views containing the complex-valued E and H fields. If ‘Normalize’ is set, the far field is normalized to 1. If ‘dB’ is set, the far field is computed in dB. If ‘NegativeTime’ is set, E and H are assumed to have exp(-iwt) time dependency; otherwise they are assume to have exp(+iwt) time dependency. If ‘MatlabOutputFile’ is given the raw far field data is also exported in Matlab format.
Plugin(NearToFarField) creates one new view.
String options:
MatlabOutputFile
Default value: "farfield.m"
Numeric options:
Wavenumber
Default value: 1
PhiStart
Default value: 0
PhiEnd
Default value: 6.28319
NumPointsPhi
Default value: 60
ThetaStart
Default value: 0
ThetaEnd
Default value: 3.14159
NumPointsTheta
Default value: 30
EView
Default value: 0
HView
Default value: 1
Normalize
Default value: 1
dB
Default value: 1
NegativeTime
Default value: 0
RFar
Default value: 0
Plugin(NearestNeighbor)
¶Plugin(NearestNeighbor) computes the distance from each point in ‘View’ to its nearest neighbor.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(NearestNeighbor) is executed in-place.
Numeric options:
View
Default value: -1
Plugin(NewView)
¶Plugin(NewView) creates a new model-based view from the current mesh, with ‘NumComp’ field components, set to value ‘Value’.
If ‘ViewTag’ is positive, force that tag for the created view. The view type is determined by ‘Type’ (NodeData or ElementData). In the case of an ElementData type, the view can be restricted to a specific physical group with a positive ‘PhysicalGroup’.
String options:
Type
Default value: "NodeData"
Numeric options:
NumComp
Default value: 1
Value
Default value: 0
ViewTag
Default value: -1
PhysicalGroup
Default value: -1
Plugin(Particles)
¶Plugin(Particles) computes the trajectory of particules in the force field given by the ‘TimeStep’-th time step of a vector view ‘View’.
The plugin takes as input a grid defined by the 3 points (‘X0’,‘Y0’,‘Z0’) (origin), (‘X1’,‘Y1’,‘Z1’) (axis of U) and (‘X2’,‘Y2’,‘Z2’) (axis of V).
The number of particles along U and V that are to be transported is set with the options ‘NumPointsU’ and ‘NumPointsV’. The equation
A2 * d^2X(t)/dt^2 + A1 * dX(t)/dt + A0 * X(t) = F
is then solved with the initial conditions X(t=0) chosen as the grid, dX/dt(t=0)=0, and with F interpolated from the vector view.
Time stepping is done using a Newmark scheme with step size ‘DT’ and ‘MaxIter’ maximum number of iterations.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Particles) creates one new list-based view containing multi-step vector points.
Numeric options:
X0
Default value: 0
Y0
Default value: 0
Z0
Default value: 0
X1
Default value: 1
Y1
Default value: 0
Z1
Default value: 0
X2
Default value: 0
Y2
Default value: 1
Z2
Default value: 0
NumPointsU
Default value: 10
NumPointsV
Default value: 1
A2
Default value: 1
A1
Default value: 0
A0
Default value: 0
DT
Default value: 0.1
MaxIter
Default value: 100
TimeStep
Default value: 0
View
Default value: -1
Plugin(Probe)
¶Plugin(Probe) gets the value of the view ‘View’ at the point (‘X’,‘Y’,‘Z’).
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Probe) creates one new view.
Numeric options:
X
Default value: 0
Y
Default value: 0
Z
Default value: 0
View
Default value: -1
Plugin(Remove)
¶Plugin(Remove) removes the marked items from the list-based view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Remove) is executed in-place.
Numeric options:
Text2D
Default value: 1
Text3D
Default value: 1
Points
Default value: 0
Lines
Default value: 0
Triangles
Default value: 0
Quadrangles
Default value: 0
Tetrahedra
Default value: 0
Hexahedra
Default value: 0
Prisms
Default value: 0
Pyramids
Default value: 0
Scalar
Default value: 1
Vector
Default value: 1
Tensor
Default value: 1
View
Default value: -1
Plugin(Scal2Tens)
¶Plugin(Scal2Tens) converts some scalar fields into a tensor field. The number of components must be given (max. 9). The new view ’NameNewView’ contains the new tensor field. If the number of a view is -1, the value of the corresponding component is 0. String options:
NameNewView
Default value: "NewView"
Numeric options:
NumberOfComponents
Default value: 9
View0
Default value: -1
View1
Default value: -1
View2
Default value: -1
View3
Default value: -1
View4
Default value: -1
View5
Default value: -1
View6
Default value: -1
View7
Default value: -1
View8
Default value: -1
Plugin(Scal2Vec)
¶Plugin(Scal2Vec) converts the scalar fields into a vectorial field. The new view ’NameNewView’ contains it. If the number of a view is -1, the value of the corresponding component of the vector field is 0. String options:
NameNewView
Default value: "NewView"
Numeric options:
ViewX
Default value: -1
ViewY
Default value: -1
ViewZ
Default value: -1
Plugin(ShowNeighborElements)
¶Plugin(ShowNeighborElements) sets visible some elements and a layer of elements around them, the other being set invisible. Numeric options:
NumLayers
Default value: 1
Element1
Default value: 0
Element2
Default value: 0
Element3
Default value: 0
Element4
Default value: 0
Element5
Default value: 0
Plugin(SimplePartition)
¶Plugin(SimplePartition) partitions the current mesh into ‘NumSlicesX’, ‘NumSlicesY’ and ‘NumSlicesZ’ slices along the X-, Y- and Z-axis, respectively. The distribtion of these slices is governed by ‘MappingX’, ‘MappingY’ and ‘MappingZ’, where ‘t’ is a normalized absissa along each direction. (Setting ‘MappingX’ to ‘t’ will thus lead to equidistant slices along the X-axis.)
The plugin creates the topology of the partitioned entities if ‘CreateTopology’ is set.
String options:
MappingX
Default value: "t"
MappingY
Default value: "t"
MappingZ
Default value: "t"
Numeric options:
NumSlicesX
Default value: 4
NumSlicesY
Default value: 1
NumSlicesZ
Default value: 1
CreateTopology
Default value: 1
Plugin(Skin)
¶Plugin(Skin) extracts the boundary (skin) of the current mesh (if ‘FromMesh’ = 1), or from the the view ‘View’ (in which case it creates a new view). If ‘View’ < 0 and ‘FromMesh’ = 0, the plugin is run on the current view.
If ‘Visible’ is set, the plugin only extracts the skin of visible entities.
Numeric options:
Visible
Default value: 1
FromMesh
Default value: 0
View
Default value: -1
Plugin(Smooth)
¶Plugin(Smooth) averages the values at the nodes of the view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Smooth) is executed in-place.
Numeric options:
View
Default value: -1
Plugin(SpanningTree)
¶Plugin(SpanningTree) builds a tree spanning every vertex of a mesh and stores it directly in the model.
The tree is constructed by starting first on the curves, then on the surfaces and finally on the volumes.
Parameters
- PhysicalVolumes: list of the physical volumes upon which the tree must be built.
- PhysicalSurfaces: list of the physical surfaces upon which the tree must be built.
- PhysicalCurves: list of the physical curves upon which the tree must be built.
- OutputPhysical: physical tag of the generated tree (-1 will select a new tag automatically).
Note - Lists must be comma separated integers and spaces are ignored.
Remark - This plugin does not overwrite a physical group.Therefore, if an existing physical tag is used in OutputPhysical, the edges of the tree will be /added/ to the specified group.
String options:
PhysicalVolumes
Default value: ""
PhysicalSurfaces
Default value: ""
PhysicalCurves
Default value: ""
Numeric options:
OutputPhysical
Default value: -1
Plugin(SphericalRaise)
¶Plugin(SphericalRaise) transforms the coordinates of the elements in the view ‘View’ using the values associated with the ‘TimeStep’-th time step.
Instead of elevating the nodes along the X, Y and Z axes as with the View[‘View’].RaiseX, View[‘View’].RaiseY and View[‘View’].RaiseZ options, the raise is applied along the radius of a sphere centered at (‘Xc’, ‘Yc’, ‘Zc’).
To produce a standard radiation pattern, set ‘Offset’ to minus the radius of the sphere the original data lives on.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(SphericalRaise) is executed in-place.
Numeric options:
Xc
Default value: 0
Yc
Default value: 0
Zc
Default value: 0
Raise
Default value: 1
Offset
Default value: 0
TimeStep
Default value: 0
View
Default value: -1
Plugin(StreamLines)
¶Plugin(StreamLines) computes stream lines from the ‘TimeStep’-th time step of a vector view ‘View’ and optionally interpolates the scalar view ‘OtherView’ on the resulting stream lines.
The plugin takes as input a grid defined by the 3 points (‘X0’,‘Y0’,‘Z0’) (origin), (‘X1’,‘Y1’,‘Z1’) (axis of U) and (‘X2’,‘Y2’,‘Z2’) (axis of V).
The number of points along U and V that are to be transported is set with the options ‘NumPointsU’ and ‘NumPointsV’. The equation
dX(t)/dt = V(x,y,z)
is then solved with the initial condition X(t=0) chosen as the grid and with V(x,y,z) interpolated on the vector view.
The time stepping scheme is a RK44 with step size ‘DT’ and ‘MaxIter’ maximum number of iterations.
If ‘TimeStep’ < 0, the plugin tries to compute streamlines of the unsteady flow.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(StreamLines) creates one new list-based view. This view contains multi-step vector points if ‘OtherView’ < 0, or single-step scalar lines if ‘OtherView’ >= 0.
Numeric options:
X0
Default value: 0
Y0
Default value: 0
Z0
Default value: 0
X1
Default value: 1
Y1
Default value: 0
Z1
Default value: 0
X2
Default value: 0
Y2
Default value: 1
Z2
Default value: 0
NumPointsU
Default value: 10
NumPointsV
Default value: 1
DT
Default value: 0.1
MaxIter
Default value: 100
TimeStep
Default value: 0
View
Default value: -1
OtherView
Default value: -1
Plugin(Summation)
¶Plugin(Summation) sums every time steps of ’Reference View’ and (every) ’Other View X’and store the result in a new view.
If ’View 0’ < 0 then the current view is selected.
If ’View 1...8’ < 0 then this view is skipped.
Views can have diffrent number of time steps
Warning: the Plugin assume that every views sharethe same mesh and that meshes do not move between time steps!
String options:
Resuling View Name
Default value: "default"
Numeric options:
View 0
Default value: -1
View 1
Default value: -1
View 2
Default value: -1
View 3
Default value: -1
View 4
Default value: -1
View 5
Default value: -1
View 6
Default value: -1
View 7
Default value: -1
Plugin(Tetrahedralize)
¶Plugin(Tetrahedralize) tetrahedralizes the points in the view ‘View’.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Tetrahedralize) creates one new list-based view.
Numeric options:
View
Default value: -1
Plugin(Transform)
¶Plugin(Transform) transforms the homogeneous node coordinates (x,y,z,1) of the elements in the view ‘View’ by the matrix
[‘A11’ ‘A12’ ‘A13’ ‘Tx’]
[‘A21’ ‘A22’ ‘A23’ ‘Ty’]
[‘A31’ ‘A32’ ‘A33’ ‘Tz’].
If ‘SwapOrientation’ is set, the orientation of the elements is reversed.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Transform) is executed in-place.
Numeric options:
A11
Default value: 1
A12
Default value: 0
A13
Default value: 0
A21
Default value: 0
A22
Default value: 1
A23
Default value: 0
A31
Default value: 0
A32
Default value: 0
A33
Default value: 1
Tx
Default value: 0
Ty
Default value: 0
Tz
Default value: 0
SwapOrientation
Default value: 0
View
Default value: -1
Plugin(Triangulate)
¶Plugin(Triangulate) triangulates the points in the view ‘View’, assuming that all the points belong to a surface that can be projected one-to-one onto a plane. Algorithm selects the old (0) or new (1) meshing algorithm.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Triangulate) creates one new list-based view.
Numeric options:
Algorithm
Default value: 1
View
Default value: -1
Plugin(VoroMetal)
¶Plugin(VoroMetal) creates microstructures using Voronoi diagrams.
String options:
SeedsFile
Default value: "seeds.txt"
Numeric options:
ComputeBestSeeds
Default value: 0
ComputeMicrostructure
Default value: 1
Plugin(Warp)
¶Plugin(Warp) transforms the elements in the view ‘View’ by adding to their node coordinates the vector field stored in the ‘TimeStep’-th time step of the view ‘OtherView’, scaled by ‘Factor’.
If ‘View’ < 0, the plugin is run on the current view.
If ‘OtherView’ < 0, the vector field is taken as the field of surface normals multiplied by the ‘TimeStep’ value in ‘View’. (The smoothing of the surface normals is controlled by the ‘SmoothingAngle’ parameter.)
Plugin(Warp) is executed in-place.
Numeric options:
Factor
Default value: 1
TimeStep
Default value: 0
SmoothingAngle
Default value: 180
View
Default value: -1
OtherView
Default value: -1
Previous: Post-processing plugins, Up: Post-processing module [Contents][Index]
General post-processing option names have the form
‘PostProcessing.string
’. Options peculiar to post-processing
views take two forms.
View.string
’, before any view is loaded;
View[n].string
’ (n = 0, 1, 2,
…), after the n-th view is loaded.
The list of all post-processing and view options is given in
Post-processing options list. See t8
: Post-processing and animations, and t9
: Plugins, for
some examples.
Next: Tutorial, Previous: Post-processing module, Up: Gmsh [Contents][Index]
This chapter describes Gmsh’s native “MSH” file format, used to store meshes and associated post-processing datasets. The MSH format exists in two flavors: ASCII and binary. The format has a version number that is independent of Gmsh’s main version number.
(Remember that for small post-processing datasets you can also use human-readable “parsed” post-processing views, as described in Post-processing commands. Such “parsed” views do not require an underlying mesh, and can therefore be easier to use in some cases.)
Next: Node ordering, Previous: File formats, Up: File formats [Contents][Index]
The MSH file format version 4 (current revision: version 4.1) contains
one mandatory section giving information about the file
($MeshFormat
), followed by several optional sections defining the
physical group names ($PhysicalName
), the elementary model
entities ($Entities
), the partitioned entities
($PartitionedEntities
), the nodes ($Nodes
), the elements
($Elements
), the periodicity relations ($Periodic
), the
ghost elements ($GhostElements
), the parametrizations
($Parametrizations
) and the post-processing datasets
($NodeData
, $ElementData
, $ElementNodeData
). The
sections reflect the underlying Gmsh data model: $Entities
store
the boundary representation of the model geometrical entities,
$Nodes
and $Elements
store mesh data classified on these
entities, and $NodeData
, $ElementData
,
$ElementNodeData
store post-processing data (views). (See
Gmsh API and Source code structure for a more detailed
description of the internal Gmsh data model.)
To represent a simple mesh, the minimal sections that should be present
in the file are $MeshFormat
, $Nodes
and
$Elements
. Nodes are assumed to be defined before elements. To
represent a mesh with the full topology (BRep) of the model and
associated physical groups, an $Entities
section should be
present before the $Nodes
section. Sections can be repeated in
the same file, and post-processing sections can be put into separate
files (e.g. one file per time step). Any section with an unrecognized
header is simply ignored: you can thus add comments in a .msh
file by putting them e.g. inside a $Comments
/$EndComments
section.
All the node, element and entity tags (their global identification
numbers) should be strictly positive. (Tag 0
is reserved for
internal use.) Important note about efficiency: tags can be "sparse",
i.e., do not have to constitute a continuous list of numbers (the format
even allows them to not be ordered). However, using sparse tags can lead
to performance degradation. For meshes, sparse indexing can15 force
Gmsh to use a map instead of a vector to access nodes and elements. The
performance hit is on speed. For post-processing datasets, which always
use vectors to access data, the performance hit is on memory. A
$NodeData
with two nodes, tagged 1 and 1000000, will allocate a
(mostly empty) vector of 1000000 elements. By default, for
non-partitioned, single file meshes, Gmsh will create files with a
continuous ordering of node and element tags, starting at 1. Detecting
if the numbering is continuous can be done easily when reading a file by
inspecting numNodes
, minNodeTag
and maxNodeTag
in
the $Nodes
section; and numElements
, minElementTag
and maxElementTag
in the $Elements
section.
In binary mode (Mesh.Binary=1
or -bin
on the command
line), all the numerical values (integer and floating point) not marked
as ASCII in the format description below are written in binary form,
using the type given between parentheses. The block structure of the
$Nodes
and $Elements
sections allows to read integer and
floating point data in each block in a single step (e.g. using
fread
in C).
The format is defined as follows:
$MeshFormat // same as MSH version 2 version(ASCII double; currently 4.1) file-type(ASCII int; 0 for ASCII mode, 1 for binary mode) data-size(ASCII int; sizeof(size_t)) < int with value one; only in binary mode, to detect endianness > $EndMeshFormat $PhysicalNames // same as MSH version 2 numPhysicalNames(ASCII int) dimension(ASCII int) physicalTag(ASCII int) "name"(127 characters max) ... $EndPhysicalNames $Entities numPoints(size_t) numCurves(size_t) numSurfaces(size_t) numVolumes(size_t) pointTag(int) X(double) Y(double) Z(double) numPhysicalTags(size_t) physicalTag(int) ... ... curveTag(int) minX(double) minY(double) minZ(double) maxX(double) maxY(double) maxZ(double) numPhysicalTags(size_t) physicalTag(int) ... numBoundingPoints(size_t) pointTag(int) ... ... surfaceTag(int) minX(double) minY(double) minZ(double) maxX(double) maxY(double) maxZ(double) numPhysicalTags(size_t) physicalTag(int) ... numBoundingCurves(size_t) curveTag(int) ... ... volumeTag(int) minX(double) minY(double) minZ(double) maxX(double) maxY(double) maxZ(double) numPhysicalTags(size_t) physicalTag(int) ... numBoundngSurfaces(size_t) surfaceTag(int) ... ... $EndEntities $PartitionedEntities numPartitions(size_t) numGhostEntities(size_t) ghostEntityTag(int) partition(int) ... numPoints(size_t) numCurves(size_t) numSurfaces(size_t) numVolumes(size_t) pointTag(int) parentDim(int) parentTag(int) numPartitions(size_t) partitionTag(int) ... X(double) Y(double) Z(double) numPhysicalTags(size_t) physicalTag(int) ... ... curveTag(int) parentDim(int) parentTag(int) numPartitions(size_t) partitionTag(int) ... minX(double) minY(double) minZ(double) maxX(double) maxY(double) maxZ(double) numPhysicalTags(size_t) physicalTag(int) ... numBoundingPoints(size_t) pointTag(int) ... ... surfaceTag(int) parentDim(int) parentTag(int) numPartitions(size_t) partitionTag(int) ... minX(double) minY(double) minZ(double) maxX(double) maxY(double) maxZ(double) numPhysicalTags(size_t) physicalTag(int) ... numBoundingCurves(size_t) curveTag(int) ... ... volumeTag(int) parentDim(int) parentTag(int) numPartitions(size_t) partitionTag(int) ... minX(double) minY(double) minZ(double) maxX(double) maxY(double) maxZ(double) numPhysicalTags(size_t) physicalTag(int) ... numBoundingSurfaces(size_t) surfaceTag(int) ... ... $EndPartitionedEntities $Nodes numEntityBlocks(size_t) numNodes(size_t) minNodeTag(size_t) maxNodeTag(size_t) entityDim(int) entityTag(int) parametric(int; 0 or 1) numNodesInBlock(size_t) nodeTag(size_t) ... x(double) y(double) z(double) < u(double; if parametric and entityDim >= 1) > < v(double; if parametric and entityDim >= 2) > < w(double; if parametric and entityDim == 3) > ... ... $EndNodes $Elements numEntityBlocks(size_t) numElements(size_t) minElementTag(size_t) maxElementTag(size_t) entityDim(int) entityTag(int) elementType(int; see below) numElementsInBlock(size_t) elementTag(size_t) nodeTag(size_t) ... ... ... $EndElements $Periodic numPeriodicLinks(size_t) entityDim(int) entityTag(int) entityTagMaster(int) numAffine(size_t) value(double) ... numCorrespondingNodes(size_t) nodeTag(size_t) nodeTagMaster(size_t) ... ... $EndPeriodic $GhostElements numGhostElements(size_t) elementTag(size_t) partitionTag(int) numGhostPartitions(size_t) ghostPartitionTag(int) ... ... $EndGhostElements $Parametrizations numCurveParam(size_t) numSurfaceParam(size_t) curveTag(int) numNodes(size_t) nodeX(double) nodeY(double) nodeZ(double) nodeU(double) ... ... surfaceTag(int) numNodes(size_t) numTriangles(size_t) nodeX(double) nodeY(double) nodeZ(double) nodeU(double) nodeV(double) curvMaxX(double) curvMaxY(double) curvMaxZ(double) curvMinX(double) curvMinY(double) curvMinZ(double) ... nodeIndex1(int) nodeIndex2(int) nodeIndex3(int) ... ... $EndParametrizations $NodeData numStringTags(ASCII int) stringTag(string) ... numRealTags(ASCII int) realTag(ASCII double) ... numIntegerTags(ASCII int) integerTag(ASCII int) ... nodeTag(int) value(double) ... ... $EndNodeData $ElementData numStringTags(ASCII int) stringTag(string) ... numRealTags(ASCII int) realTag(ASCII double) ... numIntegerTags(ASCII int) integerTag(ASCII int) ... elementTag(int) value(double) ... ... $EndElementData $ElementNodeData numStringTags(ASCII int) stringTag(string) ... numRealTags(ASCII int) realTag(ASCII double) ... numIntegerTags(ASCII int) integerTag(ASCII int) ... elementTag(int) numNodesPerElement(int) value(double) ... ... $EndElementNodeData $InterpolationScheme name(string) numElementTopologies(ASCII int) elementTopology numInterpolationMatrices(ASCII int) numRows(ASCII int) numColumns(ASCII int) value(ASCII double) ... $EndInterpolationScheme
In the format description above, elementType
is e.g.:
1
2-node line.
2
3-node triangle.
3
4-node quadrangle.
4
4-node tetrahedron.
5
8-node hexahedron.
6
6-node prism.
7
5-node pyramid.
8
3-node second order line (2 nodes associated with the vertices and 1 with the edge).
9
6-node second order triangle (3 nodes associated with the vertices and 3 with the edges).
10
9-node second order quadrangle (4 nodes associated with the vertices, 4 with the edges and 1 with the face).
11
10-node second order tetrahedron (4 nodes associated with the vertices and 6 with the edges).
12
27-node second order hexahedron (8 nodes associated with the vertices, 12 with the edges, 6 with the faces and 1 with the volume).
13
18-node second order prism (6 nodes associated with the vertices, 9 with the edges and 3 with the quadrangular faces).
14
14-node second order pyramid (5 nodes associated with the vertices, 8 with the edges and 1 with the quadrangular face).
15
1-node point.
16
8-node second order quadrangle (4 nodes associated with the vertices and 4 with the edges).
17
20-node second order hexahedron (8 nodes associated with the vertices and 12 with the edges).
18
15-node second order prism (6 nodes associated with the vertices and 9 with the edges).
19
13-node second order pyramid (5 nodes associated with the vertices and 8 with the edges).
20
9-node third order incomplete triangle (3 nodes associated with the vertices, 6 with the edges)
21
10-node third order triangle (3 nodes associated with the vertices, 6 with the edges, 1 with the face)
22
12-node fourth order incomplete triangle (3 nodes associated with the vertices, 9 with the edges)
23
15-node fourth order triangle (3 nodes associated with the vertices, 9 with the edges, 3 with the face)
24
15-node fifth order incomplete triangle (3 nodes associated with the vertices, 12 with the edges)
25
21-node fifth order complete triangle (3 nodes associated with the vertices, 12 with the edges, 6 with the face)
26
4-node third order edge (2 nodes associated with the vertices, 2 internal to the edge)
27
5-node fourth order edge (2 nodes associated with the vertices, 3 internal to the edge)
28
6-node fifth order edge (2 nodes associated with the vertices, 4 internal to the edge)
29
20-node third order tetrahedron (4 nodes associated with the vertices, 12 with the edges, 4 with the faces)
30
35-node fourth order tetrahedron (4 nodes associated with the vertices, 18 with the edges, 12 with the faces, 1 in the volume)
31
56-node fifth order tetrahedron (4 nodes associated with the vertices, 24 with the edges, 24 with the faces, 4 in the volume)
92
64-node third order hexahedron (8 nodes associated with the vertices, 24 with the edges, 24 with the faces, 8 in the volume)
93
125-node fourth order hexahedron (8 nodes associated with the vertices, 36 with the edges, 54 with the faces, 27 in the volume)
...
All the currently supported elements in the format are defined in GmshDefines.h. See Node ordering for the ordering of the nodes.
The post-processing sections ($NodeData
, $ElementData
,
$ElementNodeData
) can contain numStringTags
string tags,
numRealTags
real value tags and numIntegerTags
integer
tags. The default set of tags understood by Gmsh is as follows:
stringTag
The first is interpreted as the name of the post-processing view and the
second as the name of the interpolation scheme, as provided in the
$InterpolationScheme
section.
realTag
The first is interpreted as a time value associated with the dataset.
integerTag
The first is interpreted as a time step index (starting at 0), the second as the number of field components of the data in the view (1, 3 or 9), the third as the number of entities (nodes or elements) in the view, and the fourth as the partition index for the view data (0 for no partition).
In the $InterpolationScheme
section:
numElementTopologies
is the number of element topologies for which interpolation matrices are provided.
elementTopology
is the id tag of a given element topology: 1 for points, 2 for lines, 3 for triangles, 4 for quadrangles, 5 for tetrahedra, 6 for pyramids, 7 for prisms, 8 for hexahedra, 9 for polygons and 10 for polyhedra.
numInterpolationMatrices
is the number of interpolation matrices provided for the given element
topology. Currently you should provide 2 matrices, i.e., the matrices
that specify how to interpolate the data (they have the same meaning as
in Post-processing commands). The matrices are specified by 2
integers (numRows
and numColumns
) followed by the values,
by row.
Here is a small example of a minimal ASCII MSH4.1 file, with a mesh consisting of two quadrangles and an associated nodal scalar dataset (the comments are not part of the actual file):
$MeshFormat 4.1 0 8 MSH4.1, ASCII $EndMeshFormat $Nodes 1 6 1 6 1 entity bloc, 6 nodes total, min/max node tags: 1 and 6 2 1 0 6 2D entity (surface) 1, no parametric coordinates, 6 nodes 1 node tag #1 2 node tag #2 3 etc. 4 5 6 0. 0. 0. node #1 coordinates (0., 0., 0.) 1. 0. 0. node #2 coordinates (1., 0., 0.) 1. 1. 0. etc. 0. 1. 0. 2. 0. 0. 2. 1. 0. $EndNodes $Elements 1 2 1 2 1 entity bloc, 2 elements total, min/max element tags: 1 and 2 2 1 3 2 2D entity (surface) 1, element type 3 (4-node quad), 2 elements 1 1 2 3 4 quad tag #1, nodes 1 2 3 4 2 2 5 6 3 quad tag #2, nodes 2 5 6 3 $EndElements $NodeData 1 1 string tag: "A scalar view" the name of the view ("A scalar view") 1 1 real tag: 0.0 the time value (0.0) 3 3 integer tags: 0 the time step (0; time steps always start at 0) 1 1-component (scalar) field 6 6 associated nodal values 1 0.0 value associated with node #1 (0.0) 2 0.1 value associated with node #2 (0.1) 3 0.2 etc. 4 0.0 5 0.2 6 0.4 $EndNodeData
The 4.1 revision of the format includes the following modifications with respect to the initial 4.0 version:
unsigned long
entries have been changed to
size_t
. All the entries designating counts which were previously
encoded as int
have also been changed to size_t
. (This
only impacts binary files.)
$Entities
section is now optional.
$Nodes
section is not
mixed anymore: all the tags are given first, followed by all the
coordinates.
entityDim
and entityTag
values have been switched in
the $Nodes
and $Elements
sections (for consistency with
the ordering used elsewhere in the file and in the Gmsh API).
$Nodes
(resp. $Elements
)
section, to facilitate the detection of sparse or dense numberings when
reading the file.
$Periodic
section has been changed to always provide the
number of values in the affine transform (which can be zero, if the
transform is not provided).
The following changes are foreseen in a future revision of the MSH format:
$GhostElements
, $NodeData
, $ElementData
and
$ElementNodeData
will be reworked for greater IO efficiency, with
separation of entries by type and a block structure with predictable
sizes.
$NodeData
, $ElementData
and
$ElementNodeData
will be switched to size_t
.
Next: Legacy formats, Previous: MSH file format, Up: File formats [Contents][Index]
Historically, Gmsh first supported linear elements (lines, triangles, quadrangles, tetrahedra, prisms and hexahedra). Then, support for second and some third order elements has been added. Below we distinguish such “low order elements”, which are hardcoded (i.e. they are explicitly defined in the code), and general “high-order elements”, that have been coded in a more general fashion, theoretically valid for any order.
For all mesh and post-processing file formats, the reference elements are defined as follows.
Line: Line3: Line4: v ^ | | 0-----+-----1 --> u 0----2----1 0---2---3---1
Triangle: Triangle6: Triangle9/10: Triangle12/15: v ^ 2 | | \ 2 2 2 9 8 |`\ |`\ | \ | \ | `\ | `\ 7 6 10 (14) 7 | `\ 5 `4 | \ | \ | `\ | `\ 8 (9) 5 11 (12) (13) 6 | `\ | `\ | \ | \ 0----------1 --> u 0-----3----1 0---3---4---1 0---3---4---5---1
Quadrangle: Quadrangle8: Quadrangle9: v ^ | 3-----------2 3-----6-----2 3-----6-----2 | | | | | | | | | | | | | | | +---- | --> u 7 5 7 8 5 | | | | | | | | | | | | 0-----------1 0-----4-----1 0-----4-----1
Tetrahedron: Tetrahedron10: v . ,/ / 2 2 ,/|`\ ,/|`\ ,/ | `\ ,/ | `\ ,/ '. `\ ,6 '. `5 ,/ | `\ ,/ 8 `\ ,/ | `\ ,/ | `\ 0-----------'.--------1 --> u 0--------4--'.--------1 `\. | ,/ `\. | ,/ `\. | ,/ `\. | ,9 `\. '. ,/ `7. '. ,/ `\. |/ `\. |/ `3 `3 `\. ` w
Hexahedron: Hexahedron20: Hexahedron27: v 3----------2 3----13----2 3----13----2 |\ ^ |\ |\ |\ |\ |\ | \ | | \ | 15 | 14 |15 24 | 14 | \ | | \ 9 \ 11 \ 9 \ 20 11 \ | 7------+---6 | 7----19+---6 | 7----19+---6 | | +-- |-- | -> u | | | | |22 | 26 | 23| 0---+---\--1 | 0---+-8----1 | 0---+-8----1 | \ | \ \ | \ 17 \ 18 \ 17 25 \ 18 \ | \ \ | 10 | 12| 10 | 21 12| \| w \| \| \| \| \| 4----------5 4----16----5 4----16----5
Prism: Prism15: Prism18: w ^ | 3 3 3 ,/|`\ ,/|`\ ,/|`\ ,/ | `\ 12 | 13 12 | 13 ,/ | `\ ,/ | `\ ,/ | `\ 4------+------5 4------14-----5 4------14-----5 | | | | 8 | | 8 | | ,/|`\ | | | | | ,/|`\ | | ,/ | `\ | | | | | 15 | 16 | |,/ | `\| | | | |,/ | `\| ,| | |\ 10 | 11 10-----17-----11 ,/ | 0 | `\ | 0 | | 0 | u | ,/ `\ | v | ,/ `\ | | ,/ `\ | | ,/ `\ | | ,6 `7 | | ,6 `7 | |,/ `\| |,/ `\| |,/ `\| 1-------------2 1------9------2 1------9------2
Pyramid: Pyramid13: Pyramid14: 4 4 4 ,/|\ ,/|\ ,/|\ ,/ .'|\ ,/ .'|\ ,/ .'|\ ,/ | | \ ,/ | | \ ,/ | | \ ,/ .' | `. ,/ .' | `. ,/ .' | `. ,/ | '. \ ,7 | 12 \ ,7 | 12 \ ,/ .' w | \ ,/ .' | \ ,/ .' | \ ,/ | ^ | \ ,/ 9 | 11 ,/ 9 | 11 0----------.'--|-3 `. 0--------6-.'----3 `. 0--------6-.'----3 `. `\ | | `\ \ `\ | `\ \ `\ | `\ \ `\ .' +----`\ - \ -> v `5 .' 10 \ `5 .' 13 10 \ `\ | `\ `\ \ `\ | `\ \ `\ | `\ \ `\.' `\ `\` `\.' `\` `\.' `\` 1----------------2 1--------8-------2 1--------8-------2 `\ u
The node ordering of a higher order (possibly curved) element is compatible with the numbering of low order element (it is a generalization). We number nodes in the following order:
The numbering for internal nodes is recursive, i.e. the numbering follows that of the nodes of an embedded edge/face/volume of lower order. The higher order nodes are assumed to be equispaced. Edges and faces are numbered following the lowest order template that generates a single high-order on this edge/face. Furthermore, an edge is oriented from the node with the lowest to the highest index. The orientation of a face is such that the computed normal points outward; the starting point is the node with the lowest index.
Previous: Node ordering, Up: File formats [Contents][Index]
This section describes Gmsh’s older native file formats. Future versions of Gmsh will continue to support these formats, but we recommend that you do not use them in new applications.
Next: MSH file format version 1 (Legacy), Previous: Legacy formats, Up: Legacy formats [Contents][Index]
The MSH file format version 2 is Gmsh’s previous native mesh file format, now superseded by the format described in MSH file format. It is defined as follows:
$MeshFormat version-number file-type data-size $EndMeshFormat $PhysicalNames number-of-names physical-dimension physical-tag "physical-name" … $EndPhysicalNames $Nodes number-of-nodes node-number x-coord y-coord z-coord … $EndNodes $Elements number-of-elements elm-number elm-type number-of-tags < tag > … node-number-list … $EndElements $Periodic number-of-periodic-entities dimension entity-tag master-entity-tag number-of-nodes node-number master-node-number … $EndPeriodic $NodeData number-of-string-tags < "string-tag" > … number-of-real-tags < real-tag > … number-of-integer-tags < integer-tag > … node-number value … … $EndNodeData $ElementData number-of-string-tags < "string-tag" > … number-of-real-tags < real-tag > … number-of-integer-tags < integer-tag > … elm-number value … … $EndElementData $ElementNodeData number-of-string-tags < "string-tag" > … number-of-real-tags < real-tag > … number-of-integer-tags < integer-tag > … elm-number number-of-nodes-per-element value … … $EndElementNodeData $InterpolationScheme "name" number-of-element-topologies elm-topology number-of-interpolation-matrices num-rows num-columns value … … $EndInterpolationScheme
where
version-number
is a real number equal to 2.2
file-type
is an integer equal to 0 in the ASCII file format.
data-size
is an integer equal to the size of the floating point numbers used in the file (currently only data-size = sizeof(double) is supported).
number-of-nodes
is the number of nodes in the mesh.
node-number
is the number (index) of the n-th node in the mesh; node-number must be a postive (non-zero) integer. Note that the node-numbers do not necessarily have to form a dense nor an ordered sequence.
x-coord y-coord z-coord
are the floating point values giving the X, Y and Z coordinates of the n-th node.
number-of-elements
is the number of elements in the mesh.
elm-number
is the number (index) of the n-th element in the mesh; elm-number must be a postive (non-zero) integer. Note that the elm-numbers do not necessarily have to form a dense nor an ordered sequence.
elm-type
defines the geometrical type of the n-th element: see MSH file format.
number-of-tags
gives the number of integer tags that follow for the n-th element. By default, the first tag is the tag of the physical entity to which the element belongs; the second is the tag of the elementary model entity to which the element belongs; the third is the number of mesh partitions to which the element belongs, followed by the partition ids (negative partition ids indicate ghost cells). A zero tag is equivalent to no tag. Gmsh and most codes using the MSH 2 format require at least the first two tags (physical and elementary tags).
node-number-list
is the list of the node numbers of the n-th element. The ordering of the nodes is given in Node ordering.
number-of-string-tags
gives the number of string tags that follow. By default the first
string-tag is interpreted as the name of the post-processing view
and the second as the name of the interpolation scheme. The
interpolation scheme is provided in the $InterpolationScheme
section (see below).
number-of-real-tags
gives the number of real number tags that follow. By default the first real-tag is interpreted as a time value associated with the dataset.
number-of-integer-tags
gives the number of integer tags that follow. By default the first integer-tag is interpreted as a time step index (starting at 0), the second as the number of field components of the data in the view (1, 3 or 9), the third as the number of entities (nodes or elements) in the view, and the fourth as the partition index for the view data (0 for no partition).
number-of-nodes-per-elements
gives the number of node values for an element in an element-based view.
value
is a real number giving the value associated with a node or an
element. For NodeData
(respectively ElementData
) views,
there are ncomp values per node (resp. per element), where
ncomp is the number of field components. For
ElementNodeData
views, there are ncomp times
number-of-nodes-per-elements values per element.
number-of-element-topologies
is the number of element topologies for which interpolation matrices are provided
elm-topology
is the id tag of a given element topology: 1 for points, 2 for lines, 3 for triangles, 4 for quadrangles, 5 for tetrahedra, 6 for pyramids, 7 for prisms, 8 for hexahedra, 9 for polygons and 10 for polyhedra.
number-of-interpolation-matrices
is the number of interpolation matrices provided for the element topology elm-topology. Currently you should provide 2 matrices, i.e., the matrices that specify how to interpolate the data (they have the same meaning as in Post-processing commands). The matrices are specified by 2 integers (num-rows and num-columns) followed by the values.
Below is a small example (a mesh consisting of two quadrangles with an associated nodal scalar dataset; the comments are not part of the actual file!):
$MeshFormat 2.2 0 8 $EndMeshFormat $Nodes 6 six mesh nodes: 1 0.0 0.0 0.0 node #1: coordinates (0.0, 0.0, 0.0) 2 1.0 0.0 0.0 node #2: coordinates (1.0, 0.0, 0.0) 3 1.0 1.0 0.0 etc. 4 0.0 1.0 0.0 5 2.0 0.0 0.0 6 2.0 1.0 0.0 $EndNodes $Elements 2 two elements: 1 3 2 99 2 1 2 3 4 quad #1: type 3, physical 99, elementary 2, nodes 1 2 3 4 2 3 2 99 2 2 5 6 3 quad #2: type 3, physical 99, elementary 2, nodes 2 5 6 3 $EndElements $NodeData 1 one string tag: "A scalar view" the name of the view ("A scalar view") 1 one real tag: 0.0 the time value (0.0) 3 three integer tags: 0 the time step (0; time steps always start at 0) 1 1-component (scalar) field 6 six associated nodal values 1 0.0 value associated with node #1 (0.0) 2 0.1 value associated with node #2 (0.1) 3 0.2 etc. 4 0.0 5 0.2 6 0.4 $EndNodeData
The binary file format is similar to the ASCII format described above:
$MeshFormat version-number file-type data-size one-binary $EndMeshFormat $Nodes number-of-nodes nodes-binary $EndNodes $Elements number-of-elements element-header-binary elements-binary element-header-binary elements-binary … $EndElements [ All other sections are identical to ASCII, except that node-number, elm-number, number-of-nodes-per-element and values are written in binary format. Beware that all the $End tags must start on a new line. ]
where
version-number
is a real number equal to 2.2.
file-type
is an integer equal to 1.
data-size
has the same meaning as in the ASCII file format. Currently only data-size = sizeof(double) is supported.
one-binary
is an integer of value 1 written in binary form. This integer is used for detecting if the computer on which the binary file was written and the computer on which the file is read are of the same type (little or big endian).
Here is a pseudo C code to write one-binary:
int one = 1; fwrite(&one, sizeof(int), 1, file);
number-of-nodes
has the same meaning as in the ASCII file format.
nodes-binary
is the list of nodes in binary form, i.e., a array of number-of-nodes * (4 + 3 * data-size) bytes. For each node, the first 4 bytes contain the node number and the next (3 * data-size) bytes contain the three floating point coordinates.
Here is a pseudo C code to write nodes-binary:
for(i = 0; i < number_of_nodes; i++){ fwrite(&num_i, sizeof(int), 1, file); double xyz[3] = {node_i_x, node_i_y, node_i_z}; fwrite(xyz, sizeof(double), 3, file); }
number-of-elements
has the same meaning as in the ASCII file format.
element-header-binary
is a list of 3 integers in binary form, i.e., an array of (3 * 4) bytes: the first four bytes contain the type of the elements that follow (same as elm-type in the ASCII format), the next four contain the number of elements that follow, and the last four contain the number of tags per element (same as number-of-tags in the ASCII format).
Here is a pseudo C code to write element-header-binary:
int header[3] = {elm_type, num_elm_follow, num_tags}; fwrite(header, sizeof(int), 3, file);
elements-binary
is a list of elements in binary form, i.e., an array of “number of elements that follow” * (4 + number-of-tags * 4 + #node-number-list * 4) bytes. For each element, the first four bytes contain the element number, the next (number-of-tags * 4) contain the tags, and the last (#node-number-list * 4) contain the node indices.
Here is a pseudo C code to write elements-binary for triangles with the 2 standard tags (the physical and elementary regions):
for(i = 0; i < number_of_triangles; i++){ int data[6] = {num_i, physical, elementary, node_i_1, node_i_2, node_i_3}; fwrite(data, sizeof(int), 6, file); }
Next: POS ASCII file format (Legacy), Previous: MSH file format version 2 (Legacy), Up: Legacy formats [Contents][Index]
The MSH file format version 1 is Gmsh’s original native mesh file format, now superseded by the format described in MSH file format. It is defined as follows:
$NOD number-of-nodes node-number x-coord y-coord z-coord … $ENDNOD $ELM number-of-elements elm-number elm-type reg-phys reg-elem number-of-nodes node-number-list … $ENDELM
where
number-of-nodes
is the number of nodes in the mesh.
node-number
is the number (index) of the n-th node in the mesh; node-number must be a postive (non-zero) integer. Note that the node-numbers do not necessarily have to form a dense nor an ordered sequence.
x-coord y-coord z-coord
are the floating point values giving the X, Y and Z coordinates of the n-th node.
number-of-elements
is the number of elements in the mesh.
elm-number
is the number (index) of the n-th element in the mesh; elm-number must be a postive (non-zero) integer. Note that the elm-numbers do not necessarily have to form a dense nor an ordered sequence.
elm-type
defines the geometrical type of the n-th element:
1
2-node line.
2
3-node triangle.
3
4-node quadrangle.
4
4-node tetrahedron.
5
8-node hexahedron.
6
6-node prism.
7
5-node pyramid.
8
3-node second order line (2 nodes associated with the vertices and 1 with the edge).
9
6-node second order triangle (3 nodes associated with the vertices and 3 with the edges).
10
9-node second order quadrangle (4 nodes associated with the vertices, 4 with the edges and 1 with the face).
11
10-node second order tetrahedron (4 nodes associated with the vertices and 6 with the edges).
12
27-node second order hexahedron (8 nodes associated with the vertices, 12 with the edges, 6 with the faces and 1 with the volume).
13
18-node second order prism (6 nodes associated with the vertices, 9 with the edges and 3 with the quadrangular faces).
14
14-node second order pyramid (5 nodes associated with the vertices, 8 with the edges and 1 with the quadrangular face).
15
1-node point.
16
8-node second order quadrangle (4 nodes associated with the vertices and 4 with the edges).
17
20-node second order hexahedron (8 nodes associated with the vertices and 12 with the edges).
18
15-node second order prism (6 nodes associated with the vertices and 9 with the edges).
19
13-node second order pyramid (5 nodes associated with the vertices and 8 with the edges).
See below for the ordering of the nodes.
reg-phys
is the tag of the physical entity to which the element belongs; reg-phys must be a postive integer, or zero. If reg-phys is equal to zero, the element is considered not to belong to any physical entity.
reg-elem
is the tag of the elementary entity to which the element belongs; reg-elem must be a postive (non-zero) integer.
number-of-nodes
is the number of nodes for the n-th element. This is redundant, but kept for backward compatibility.
node-number-list
is the list of the number-of-nodes node numbers of the n-th element. The ordering of the nodes is given in Node ordering.
Next: POS binary file format (Legacy), Previous: MSH file format version 1 (Legacy), Up: Legacy formats [Contents][Index]
The POS ASCII file is Gmsh’s old native post-processing format, now superseded by the format described in MSH file format. It is defined as follows:
$PostFormat 1.4 file-type data-size $EndPostFormat $View view-name nb-time-steps nb-scalar-points nb-vector-points nb-tensor-points nb-scalar-lines nb-vector-lines nb-tensor-lines nb-scalar-triangles nb-vector-triangles nb-tensor-triangles nb-scalar-quadrangles nb-vector-quadrangles nb-tensor-quadrangles nb-scalar-tetrahedra nb-vector-tetrahedra nb-tensor-tetrahedra nb-scalar-hexahedra nb-vector-hexahedra nb-tensor-hexahedra nb-scalar-prisms nb-vector-prisms nb-tensor-prisms nb-scalar-pyramids nb-vector-pyramids nb-tensor-pyramids nb-scalar-lines2 nb-vector-lines2 nb-tensor-lines2 nb-scalar-triangles2 nb-vector-triangles2 nb-tensor-triangles2 nb-scalar-quadrangles2 nb-vector-quadrangles2 nb-tensor-quadrangles2 nb-scalar-tetrahedra2 nb-vector-tetrahedra2 nb-tensor-tetrahedra2 nb-scalar-hexahedra2 nb-vector-hexahedra2 nb-tensor-hexahedra2 nb-scalar-prisms2 nb-vector-prisms2 nb-tensor-prisms2 nb-scalar-pyramids2 nb-vector-pyramids2 nb-tensor-pyramids2 nb-text2d nb-text2d-chars nb-text3d nb-text3d-chars time-step-values < scalar-point-value > … < vector-point-value > … < tensor-point-value > … < scalar-line-value > … < vector-line-value > … < tensor-line-value > … < scalar-triangle-value > … < vector-triangle-value > … < tensor-triangle-value > … < scalar-quadrangle-value > … < vector-quadrangle-value > … < tensor-quadrangle-value > … < scalar-tetrahedron-value > … < vector-tetrahedron-value > … < tensor-tetrahedron-value > … < scalar-hexahedron-value > … < vector-hexahedron-value > … < tensor-hexahedron-value > … < scalar-prism-value > … < vector-prism-value > … < tensor-prism-value > … < scalar-pyramid-value > … < vector-pyramid-value > … < tensor-pyramid-value > … < scalar-line2-value > … < vector-line2-value > … < tensor-line2-value > … < scalar-triangle2-value > … < vector-triangle2-value > … < tensor-triangle2-value > … < scalar-quadrangle2-value > … < vector-quadrangle2-value > … < tensor-quadrangle2-value > … < scalar-tetrahedron2-value > … < vector-tetrahedron2-value > … < tensor-tetrahedron2-value > … < scalar-hexahedron2-value > … < vector-hexahedron2-value > … < tensor-hexahedron2-value > … < scalar-prism2-value > … < vector-prism2-value > … < tensor-prism2-value > … < scalar-pyramid2-value > … < vector-pyramid2-value > … < tensor-pyramid2-value > … < text2d > … < text2d-chars > … < text3d > … < text3d-chars > … $EndView
where
file-type
is an integer equal to 0 in the ASCII file format.
data-size
is an integer equal to the size of the floating point numbers used in the file (usually, data-size = sizeof(double)).
view-name
is a string containing the name of the view (max. 256 characters).
nb-time-steps
is an integer giving the number of time steps in the view.
nb-scalar-points
nb-vector-points
…
are integers giving the number of scalar points, vector points, …, in the view.
nb-text2d
nb-text3d
are integers giving the number of 2D and 3D text strings in the view.
nb-text2d-chars
nb-text3d-chars
are integers giving the total number of characters in the 2D and 3D strings.
time-step-values
is a list of nb-time-steps double precision numbers giving the value of the time (or any other variable) for which an evolution was saved.
scalar-point-value
vector-point-value
…
are lists of double precision numbers giving the node coordinates and the values associated with the nodes of the nb-scalar-points scalar points, nb-vector-points vector points, …, for each of the time-step-values.
For example, vector-triangle-value is defined as:
coord1-node1 coord1-node2 coord1-node3 coord2-node1 coord2-node2 coord2-node3 coord3-node1 coord3-node2 coord3-node3 comp1-node1-time1 comp2-node1-time1 comp3-node1-time1 comp1-node2-time1 comp2-node2-time1 comp3-node2-time1 comp1-node3-time1 comp2-node3-time1 comp3-node3-time1 comp1-node1-time2 comp2-node1-time2 comp3-node1-time2 comp1-node2-time2 comp2-node2-time2 comp3-node2-time2 comp1-node3-time2 comp2-node3-time2 comp3-node3-time2 …
The ordering of the nodes is given in Node ordering.
text2d
is a list of 4 double precision numbers:
coord1 coord2 style index
where coord1 and coord2 give the X-Y position of the 2D string in screen coordinates (measured from the top-left corner of the window) and where index gives the starting index of the string in text2d-chars. If coord1 (respectively coord2) is negative, the position is measured from the right (respectively bottom) edge of the window. If coord1 (respectively coord2) is larger than 99999, the string is centered horizontally (respectively vertically). If style is equal to zero, the text is aligned bottom-left and displayed using the default font and size. Otherwise, style is converted into an integer whose eight lower bits give the font size, whose eight next bits select the font (the index corresponds to the position in the font menu in the GUI), and whose eight next bits define the text alignment (0=bottom-left, 1=bottom-center, 2=bottom-right, 3=top-left, 4=top-center, 5=top-right, 6=center-left, 7=center-center, 8=center-right).
text2d-chars
is a list of nb-text2d-chars characters. Substrings are separated with
the null ‘\0
’ character.
text3d
is a list of 5 double precision numbers
coord1 coord2 coord3 style index
where coord1, coord2 and coord3 give the XYZ coordinates of the string in model (real world) coordinates, index gives the starting index of the string in text3d-chars, and style has the same meaning as in text2d.
text3d-chars
is a list of nb-text3d-chars chars. Substrings are separated with the
null ‘\0
’ character.
Previous: POS ASCII file format (Legacy), Up: Legacy formats [Contents][Index]
The POS binary file format is the same as the POS ASCII file format described in POS ASCII file format (Legacy), except that:
Here is a pseudo C code to write a post-processing file in binary format:
int one = 1; fprintf(file, "$PostFormat\n"); fprintf(file, "%g %d %d\n", 1.4, 1, sizeof(double)); fprintf(file, "$EndPostFormat\n"); fprintf(file, "$View\n"); fprintf(file, "%s %d " "%d %d %d %d %d %d %d %d %d " "%d %d %d %d %d %d %d %d %d " "%d %d %d %d %d %d %d %d %d " "%d %d %d %d %d %d %d %d %d " "%d %d %d %d %d %d %d %d %d " "%d %d %d %d\n", view-name, nb-time-steps, nb-scalar-points, nb-vector-points, nb-tensor-points, nb-scalar-lines, nb-vector-lines, nb-tensor-lines, nb-scalar-triangles, nb-vector-triangles, nb-tensor-triangles, nb-scalar-quadrangles, nb-vector-quadrangles, nb-tensor-quadrangles, nb-scalar-tetrahedra, nb-vector-tetrahedra, nb-tensor-tetrahedra, nb-scalar-hexahedra, nb-vector-hexahedra, nb-tensor-hexahedra, nb-scalar-prisms, nb-vector-prisms, nb-tensor-prisms, nb-scalar-pyramids, nb-vector-pyramids, nb-tensor-pyramids, nb-scalar-lines2, nb-vector-lines2, nb-tensor-lines2, nb-scalar-triangles2, nb-vector-triangles2, nb-tensor-triangles2, nb-scalar-quadrangles2, nb-vector-quadrangles2, nb-tensor-quadrangles2, nb-scalar-tetrahedra2, nb-vector-tetrahedra2, nb-tensor-tetrahedra2, nb-scalar-hexahedra2, nb-vector-hexahedra2, nb-tensor-hexahedra2, nb-scalar-prisms2, nb-vector-prisms2, nb-tensor-prisms2, nb-scalar-pyramids2, nb-vector-pyramids2, nb-tensor-pyramids2, nb-text2d, nb-text2d-chars, nb-text3d, nb-text3d-chars); fwrite(&one, sizeof(int), 1, file); fwrite(time-step-values, sizeof(double), nb-time-steps, file); fwrite(all-scalar-point-values, sizeof(double), ..., file); ... fprintf(file, "\n$EndView\n");
In this pseudo-code, all-scalar-point-values is the array of double precision numbers containing all the scalar-point-value lists, put one after each other in order to form a long array of doubles. The principle is the same for all other kinds of values.
Next: Options, Previous: File formats, Up: Gmsh [Contents][Index]
The following tutorials introduce new features gradually, starting with
t1
: Geometry basics, elementary entities, physical groups. The corresponding files are available in the
tutorial
directory of the Gmsh distribution. The files starting with t
introduce features available both in .geo
scripts and through the
Gmsh API. The files starting with x
introduce features that
are only available via the API.
To learn how to run Gmsh on your computer, see Running Gmsh on your system. Screencasts that show how to use the GUI are available on https://gmsh.info/screencasts/. To learn how to run the C++, C, Python and Julia API examples, see the respective subdirectories in tutorial.
t1
: Geometry basics, elementary entities, physical groupst2
: Transformations, extruded geometries, volumest3
: Extruded meshes, ONELAB parameters, optionst4
: Built-in functions, holes in surfaces, annotations, entity colorst5
: Mesh sizes, macros, loops, holes in volumest6
: Transfinite meshest7
: Background meshest8
: Post-processing and animationst9
: Pluginst10
: Mesh size fieldst11
: Unstructured quadrangular meshest12
: Cross-patch meshing with compoundst13
: Remeshing an STL file without an underlying CAD modelt14
: Homology and cohomology computationt15
: Embedded points, lines and surfacest16
: Constructive Solid Geometry, OpenCASCADE geometry kernelt17
: Anisotropic background mesht18
: Periodic meshest19
: Thrusections, fillets, pipes, mesh size from curvaturet20
: STEP import and manipulation, geometry partitioningt21
: Mesh partitioningx1
: Geometry and mesh datax2
: Mesh import, discrete entities, hybrid models, terrain meshingx3
: Post-processing data import: list-basedx4
: Post-processing data import: model-based
Next: t2
: Transformations, extruded geometries, volumes, Previous: Tutorial, Up: Tutorial [Contents][Index]
t1
: Geometry basics, elementary entities, physical groupsSee t1.geo. Also available in C++ (t1.cpp), C (t1.c), Python (t1.py) and Julia (t1.jl).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 1 // // Geometry basics, elementary entities, physical groups // // ----------------------------------------------------------------------------- // The simplest construction in Gmsh's scripting language is the // `affectation'. The following command defines a new variable `lc': lc = 1e-2; // This variable can then be used in the definition of Gmsh's simplest // `elementary entity', a `Point'. A Point is uniquely identified by a tag (a // strictly positive integer; here `1') and defined by a list of four numbers: // three coordinates (X, Y and Z) and the target mesh size (lc) close to the // point: Point(1) = {0, 0, 0, lc}; // The distribution of the mesh element sizes will then be obtained by // interpolation of these mesh sizes throughout the geometry. Another method to // specify mesh sizes is to use general mesh size Fields (see `t10.geo'). A // particular case is the use of a background mesh (see `t7.geo'). // If no target mesh size of provided, a default uniform coarse size will be // used for the model, based on the overall model size. // We can then define some additional points. All points should have different // tags: Point(2) = {.1, 0, 0, lc}; Point(3) = {.1, .3, 0, lc}; Point(4) = {0, .3, 0, lc}; // Curves are Gmsh's second type of elementary entities, and, amongst curves, // straight lines are the simplest. A straight line is identified by a tag and // is defined by a list of two point tags. In the commands below, for example, // the line 1 starts at point 1 and ends at point 2. // // Note that curve tags are separate from point tags - hence we can reuse tag // `1' for our first curve. And as a general rule, elementary entity tags in // Gmsh have to be unique per geometrical dimension. Line(1) = {1, 2}; Line(2) = {3, 2}; Line(3) = {3, 4}; Line(4) = {4, 1}; // The third elementary entity is the surface. In order to define a simple // rectangular surface from the four curves defined above, a curve loop has // first to be defined. A curve loop is also identified by a tag (unique amongst // curve loops) and defined by an ordered list of connected curves, a sign being // associated with each curve (depending on the orientation of the curve to form // a loop): Curve Loop(1) = {4, 1, -2, 3}; // We can then define the surface as a list of curve loops (only one here, // representing the external contour, since there are no holes--see `t4.geo' for // an example of a surface with a hole): Plane Surface(1) = {1}; // At this level, Gmsh knows everything to display the rectangular surface 1 and // to mesh it. An optional step is needed if we want to group elementary // geometrical entities into more meaningful groups, e.g. to define some // mathematical ("domain", "boundary"), functional ("left wing", "fuselage") or // material ("steel", "carbon") properties. // // Such groups are called "Physical Groups" in Gmsh. By default, if physical // groups are defined, Gmsh will export in output files only mesh elements that // belong to at least one physical group. (To force Gmsh to save all elements, // whether they belong to physical groups or not, set `Mesh.SaveAll=1;', or // specify `-save_all' on the command line.) Physical groups are also identified // by tags, i.e. strictly positive integers, that should be unique per dimension // (0D, 1D, 2D or 3D). Physical groups can also be given names. // // Here we define a physical curve that groups the left, bottom and right curves // in a single group (with prescribed tag 5); and a physical surface with name // "My surface" (with an automatic tag) containing the geometrical surface 1: Physical Curve(5) = {1, 2, 4}; Physical Surface("My surface") = {1}; // Now that the geometry is complete, you can // - either open this file with Gmsh and select `2D' in the `Mesh' module to // create a mesh; then select `Save' to save it to disk in the default format // (or use `File->Export' to export in other formats); // - or run `gmsh t1.geo -2` to mesh in batch mode on the command line. // You could also uncomment the following lines in this script: // // Mesh 2; // Save "t1.msh"; // // which would lead Gmsh to mesh and save the mesh every time the file is // parsed. (To simply parse the file from the command line, you can use `gmsh // t1.geo -') // By default, Gmsh saves meshes in the latest version of the Gmsh mesh file // format (the `MSH' format). You can save meshes in other mesh formats by // specifying a filename with a different extension in the GUI, on the command // line or in scripts. For example // // Save "t1.unv"; // // will save the mesh in the UNV format. You can also save the mesh in older // versions of the MSH format: // // - In the GUI: open `File->Export', enter your `filename.msh' and then pick // the version in the dropdown menu. // - On the command line: use the `-format' option (e.g. `gmsh file.geo -format // msh2 -2'). // - In a `.geo' script: add `Mesh.MshFileVersion = x.y;' for any version // number `x.y'. // - As an alternative method, you can also not specify the format explicitly, // and just choose a filename with the `.msh2' or `.msh4' extension. // Note that starting with Gmsh 3.0, models can be built using other geometry // kernels than the default built-in kernel. By specifying // // SetFactory("OpenCASCADE"); // // any subsequent command in the `.geo' file would be handled by the OpenCASCADE // geometry kernel instead of the built-in kernel. Different geometry kernels // have different features. With OpenCASCADE, instead of defining the surface by // successively defining 4 points, 4 curves and 1 curve loop, one can define the // rectangular surface directly with // // Rectangle(2) = {.2, 0, 0, .1, .3}; // // The underlying curves and points could be accessed with the `Boundary' or // `CombinedBoundary' operators. // // See e.g. `t16.geo', `t18.geo', `t19.geo' or `t20.geo' for complete examples // based on OpenCASCADE, and `demos/boolean' for more.
Next: t3
: Extruded meshes, ONELAB parameters, options, Previous: t1
: Geometry basics, elementary entities, physical groups, Up: Tutorial [Contents][Index]
t2
: Transformations, extruded geometries, volumesSee t2.geo. Also available in C++ (t2.cpp), Python (t2.py) and Julia (t2.jl).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 2 // // Transformations, extruded geometries, volumes // // ----------------------------------------------------------------------------- // We first include the previous tutorial file, in order to use it as a basis // for this one. Including a file is equivalent to copy-pasting its contents: Include "t1.geo"; // We can then add new points and curves in the same way as we did in `t1.geo': Point(5) = {0, .4, 0, lc}; Line(5) = {4, 5}; // Gmsh also provides tools to transform (translate, rotate, etc.) // elementary entities or copies of elementary entities. For example, point // 5 can be moved by 0.02 to the left with: Translate {-0.02, 0, 0} { Point{5}; } // And it can be further rotated by -Pi/4 around (0, 0.3, 0) (with the rotation // along the z axis) with: Rotate {{0,0,1}, {0,0.3,0}, -Pi/4} { Point{5}; } // Note that there are no units in Gmsh: coordinates are just numbers - it's up // to the user to associate a meaning to them. // Point 3 can be duplicated and translated by 0.05 along the y axis: Translate {0, 0.05, 0} { Duplicata{ Point{3}; } } // This command created a new point with an automatically assigned tag. This tag // can be obtained using the graphical user interface by hovering the mouse over // the point: in this case, the new point has tag `6'. Line(7) = {3, 6}; Line(8) = {6, 5}; Curve Loop(10) = {5,-8,-7,3}; Plane Surface(11) = {10}; // To automate the workflow, instead of using the graphical user interface to // obtain the tags of newly created entities, one can use the return value of // the transformation commands directly. For example, the `Translate' command // returns a list containing the tags of the translated entities. Let's // translate copies of the two surfaces 1 and 11 to the right with the following // command: my_new_surfs[] = Translate {0.12, 0, 0} { Duplicata{ Surface{1, 11}; } }; // my_new_surfs[] (note the square brackets, and the `;' at the end of the // command) denotes a list, which contains the tags of the two new surfaces // (check `Tools->Message console' to see the message): Printf("New surfaces '%g' and '%g'", my_new_surfs[0], my_new_surfs[1]); // In Gmsh lists use square brackets for their definition (mylist[] = {1, 2, // 3};) as well as to access their elements (myotherlist[] = {mylist[0], // mylist[2]}; mythirdlist[] = myotherlist[];), with list indexing starting at // 0. To get the size of a list, use the hash (pound): len = #mylist[]. // // Note that parentheses can also be used instead of square brackets, so that we // could also write `myfourthlist() = {mylist(0), mylist(1)};'. // Volumes are the fourth type of elementary entities in Gmsh. In the same way // one defines curve loops to build surfaces, one has to define surface loops // (i.e. `shells') to build volumes. The following volume does not have holes // and thus consists of a single surface loop: Point(100) = {0., 0.3, 0.12, lc}; Point(101) = {0.1, 0.3, 0.12, lc}; Point(102) = {0.1, 0.35, 0.12, lc}; xyz[] = Point{5}; // Get coordinates of point 5 Point(103) = {xyz[0], xyz[1], 0.12, lc}; Line(110) = {4, 100}; Line(111) = {3, 101}; Line(112) = {6, 102}; Line(113) = {5, 103}; Line(114) = {103, 100}; Line(115) = {100, 101}; Line(116) = {101, 102}; Line(117) = {102, 103}; Curve Loop(118) = {115, -111, 3, 110}; Plane Surface(119) = {118}; Curve Loop(120) = {111, 116, -112, -7}; Plane Surface(121) = {120}; Curve Loop(122) = {112, 117, -113, -8}; Plane Surface(123) = {122}; Curve Loop(124) = {114, -110, 5, 113}; Plane Surface(125) = {124}; Curve Loop(126) = {115, 116, 117, 114}; Plane Surface(127) = {126}; Surface Loop(128) = {127, 119, 121, 123, 125, 11}; Volume(129) = {128}; // When a volume can be extruded from a surface, it is usually easier to use the // `Extrude' command directly instead of creating all the points, curves and // surfaces by hand. For example, the following command extrudes the surface 11 // along the z axis and automatically creates a new volume (as well as all the // needed points, curves and surfaces): Extrude {0, 0, 0.12} { Surface{my_new_surfs[1]}; } // The following command permits to manually assign a mesh size to some of the // new points: MeshSize {103, 105, 109, 102, 28, 24, 6, 5} = lc * 3; // We finally group volumes 129 and 130 in a single physical group with tag `1' // and name "The volume": Physical Volume("The volume", 1) = {129,130}; // Note that, if the transformation tools are handy to create complex // geometries, it is also sometimes useful to generate the `flat' geometry, with // an explicit representation of all the elementary entities. // // With the built-in geometry kernel, this can be achieved with `File->Export' by // selecting the `Gmsh Unrolled GEO' format, or by adding // // Save "file.geo_unrolled"; // // in the script. It can also be achieved with `gmsh t2.geo -0' on the command // line. // // With the OpenCASCADE geometry kernel, unrolling the geometry can be achieved // with `File->Export' by selecting the `OpenCASCADE BRep' format, or by adding // // Save "file.brep"; // // in the script. (OpenCASCADE geometries can also be exported to STEP.) // It is important to note that Gmsh never translates geometry data into a // common representation: all the operations on a geometrical entity are // performed natively with the associated geometry kernel. Consequently, one // cannot export a geometry constructed with the built-in kernel as an // OpenCASCADE BRep file; or export an OpenCASCADE model as an Unrolled GEO // file.
Next: t4
: Built-in functions, holes in surfaces, annotations, entity colors, Previous: t2
: Transformations, extruded geometries, volumes, Up: Tutorial [Contents][Index]
t3
: Extruded meshes, ONELAB parameters, optionsSee t3.geo. Also available in C++ (t3.cpp), Python (t3.py) and Julia (t3.jl).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 3 // // Extruded meshes, ONELAB parameters, options // // ----------------------------------------------------------------------------- // Again, we start by including the first tutorial: Include "t1.geo"; // As in `t2.geo', we plan to perform an extrusion along the z axis. But here, // instead of only extruding the geometry, we also want to extrude the 2D // mesh. This is done with the same `Extrude' command, but by specifying element // 'Layers' (2 layers in this case, the first one with 8 subdivisions and the // second one with 2 subdivisions, both with a height of h/2): h = 0.1; Extrude {0,0,h} { Surface{1}; Layers{ {8,2}, {0.5,1} }; } // The extrusion can also be performed with a rotation instead of a translation, // and the resulting mesh can be recombined into prisms (we use only one layer // here, with 7 subdivisions). All rotations are specified by an axis direction // ({0,1,0}), an axis point ({-0.1,0,0.1}) and a rotation angle (-Pi/2): Extrude { {0,1,0} , {-0.1,0,0.1} , -Pi/2 } { Surface{28}; Layers{7}; Recombine; } // Using the built-in geometry kernel, only rotations with angles < Pi are // supported. To do a full turn, you will thus need to apply at least 3 // rotations. The OpenCASCADE geometry kernel does not have this limitation. // Note that a translation ({-2*h,0,0}) and a rotation ({1,0,0}, {0,0.15,0.25}, // Pi/2) can also be combined to form a "twist". Here the angle is specified as // a ONELAB parameter, using the `DefineConstant' syntax. ONELAB parameters can // be modified interactively in the GUI, and can be exchanged with other codes // connected to the same ONELAB database: DefineConstant[ angle = {90, Min 0, Max 120, Step 1, Name "Parameters/Twisting angle"} ]; // In more details, `DefineConstant' allows you to assign the value of the // ONELAB parameter "Parameters/Twisting angle" to the variable `angle'. If the // ONELAB parameter does not exist in the database, `DefineConstant' will create // it and assign the default value `90'. Moreover, if the variable `angle' was // defined before the call to `DefineConstant', the `DefineConstant' call would // simply be skipped. This allows to build generic parametric models, whose // parameters can be frozen from the outside - the parameters ceasing to be // "parameters". // // An interesting use of this feature is in conjunction with the `-setnumber // name value' command line switch, which defines a variable `name' with value // `value'. Calling `gmsh t2.geo -setnumber angle 30' would define `angle' // before the `DefineConstant', making `t2.geo' non-parametric // ("Parameters/Twisting angle" will not be created in the ONELAB database and // will not be available for modification in the graphical user interface). out[] = Extrude { {-2*h,0,0}, {1,0,0} , {0,0.15,0.25} , angle * Pi / 180 } { Surface{50}; Layers{10}; Recombine; }; // In this last extrusion command we retrieved the volume number // programmatically by using the return value (a list) of the `Extrude' // command. This list contains the "top" of the extruded surface (in `out[0]'), // the newly created volume (in `out[1]') and the tags of the lateral surfaces // (in `out[2]', `out[3]', ...). // We can then define a new physical volume (with tag 101) to group all the // elementary volumes: Physical Volume(101) = {1, 2, out[1]}; // Let us now change some options... Since all interactive options are // accessible in Gmsh's scripting language, we can for example make point tags // visible or redefine some colors directly in the input file: Geometry.PointNumbers = 1; Geometry.Color.Points = Orange; General.Color.Text = White; Mesh.Color.Points = {255, 0, 0}; // Note that all colors can be defined literally or numerically, i.e. // `Mesh.Color.Points = Red' is equivalent to `Mesh.Color.Points = {255,0,0}'; // and also note that, as with user-defined variables, the options can be used // either as right or left hand sides, so that the following command will set // the surface color to the same color as the points: Geometry.Color.Surfaces = Geometry.Color.Points; // You can use the `Help->Current Options and Workspace' menu to see the current // values of all options. To save all the options in a file, use // `File->Export->Gmsh Options'. To associate the current options with the // current file use `File->Save Model Options'. To save the current options for // all future Gmsh sessions use `File->Save Options As Default'.
Next: t5
: Mesh sizes, macros, loops, holes in volumes, Previous: t3
: Extruded meshes, ONELAB parameters, options, Up: Tutorial [Contents][Index]
t4
: Built-in functions, holes in surfaces, annotations, entity colorsSee t4.geo. Also available in C++ (t4.cpp), Python (t4.py) and Julia (t4.jl).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 4 // // Built-in functions, holes in surfaces, annotations, entity colors // // ----------------------------------------------------------------------------- // As usual, we start by defining some variables: cm = 1e-02; e1 = 4.5 * cm; e2 = 6 * cm / 2; e3 = 5 * cm / 2; h1 = 5 * cm; h2 = 10 * cm; h3 = 5 * cm; h4 = 2 * cm; h5 = 4.5 * cm; R1 = 1 * cm; R2 = 1.5 * cm; r = 1 * cm; Lc1 = 0.01; Lc2 = 0.003; // We can use all the usual mathematical functions (note the capitalized first // letters), plus some useful functions like Hypot(a, b) := Sqrt(a^2 + b^2): ccos = (-h5*R1 + e2 * Hypot(h5, Hypot(e2, R1))) / (h5^2 + e2^2); ssin = Sqrt(1 - ccos^2); // Then we define some points and some lines using these variables: Point(1) = {-e1-e2, 0 , 0, Lc1}; Point(2) = {-e1-e2, h1 , 0, Lc1}; Point(3) = {-e3-r , h1 , 0, Lc2}; Point(4) = {-e3-r , h1+r , 0, Lc2}; Point(5) = {-e3 , h1+r , 0, Lc2}; Point(6) = {-e3 , h1+h2, 0, Lc1}; Point(7) = { e3 , h1+h2, 0, Lc1}; Point(8) = { e3 , h1+r , 0, Lc2}; Point(9) = { e3+r , h1+r , 0, Lc2}; Point(10)= { e3+r , h1 , 0, Lc2}; Point(11)= { e1+e2, h1 , 0, Lc1}; Point(12)= { e1+e2, 0 , 0, Lc1}; Point(13)= { e2 , 0 , 0, Lc1}; Point(14)= { R1 / ssin, h5+R1*ccos, 0, Lc2}; Point(15)= { 0 , h5 , 0, Lc2}; Point(16)= {-R1 / ssin, h5+R1*ccos, 0, Lc2}; Point(17)= {-e2 , 0.0 , 0, Lc1}; Point(18)= {-R2 , h1+h3 , 0, Lc2}; Point(19)= {-R2 , h1+h3+h4, 0, Lc2}; Point(20)= { 0 , h1+h3+h4, 0, Lc2}; Point(21)= { R2 , h1+h3+h4, 0, Lc2}; Point(22)= { R2 , h1+h3 , 0, Lc2}; Point(23)= { 0 , h1+h3 , 0, Lc2}; Point(24)= { 0, h1+h3+h4+R2, 0, Lc2}; Point(25)= { 0, h1+h3-R2, 0, Lc2}; Line(1) = {1 , 17}; Line(2) = {17, 16}; // Gmsh provides other curve primitives than straight lines: splines, B-splines, // circle arcs, ellipse arcs, etc. Here we define a new circle arc, starting at // point 14 and ending at point 16, with the circle's center being the point 15: Circle(3) = {14,15,16}; // Note that, in Gmsh, circle arcs should always be smaller than Pi. The // OpenCASCADE geometry kernel does not have this limitation. // We can then define additional lines and circles, as well as a new surface: Line(4) = {14, 13}; Line(5) = {13, 12}; Line(6) = {12, 11}; Line(7) = {11, 10}; Circle(8) = {8, 9, 10}; Line(9) = {8, 7}; Line(10) = {7, 6}; Line(11) = {6, 5}; Circle(12) = {3, 4, 5}; Line(13) = {3, 2}; Line(14) = {2, 1}; Line(15) = {18, 19}; Circle(16) = {21, 20, 24}; Circle(17) = {24, 20, 19}; Circle(18) = {18, 23, 25}; Circle(19) = {25, 23, 22}; Line(20) = {21,22}; Curve Loop(21) = {17, -15, 18, 19, -20, 16}; Plane Surface(22) = {21}; // But we still need to define the exterior surface. Since this surface has a // hole, its definition now requires two curves loops: Curve Loop(23) = {11, -12, 13, 14, 1, 2, -3, 4, 5, 6, 7, -8, 9, 10}; Plane Surface(24) = {23, 21}; // As a general rule, if a surface has N holes, it is defined by N+1 curve loops: // the first loop defines the exterior boundary; the other loops define the // boundaries of the holes. // Finally, we can add some comments by embedding a post-processing view // containing some strings: View "comments" { // Add a text string in window coordinates, 10 pixels from the left and 10 // pixels from the bottom, using the `StrCat' function to concatenate strings: T2(10, -10, 0){ StrCat("Created on ", Today, " with Gmsh") }; // Add a text string in model coordinates centered at (X,Y,Z) = (0, 0.11, 0): T3(0, 0.11, 0, TextAttributes("Align", "Center", "Font", "Helvetica")){ "Hole" }; // If a string starts with `file://', the rest is interpreted as an image // file. For 3D annotations, the size in model coordinates can be specified // after a `@' symbol in the form `widthxheight' (if one of `width' or // `height' is zero, natural scaling is used; if both are zero, original image // dimensions in pixels are used): T3(0, 0.09, 0, TextAttributes("Align", "Center")){ "file://t4_image.png@0.01x0" }; // The 3D orientation of the image can be specified by proving the direction // of the bottom and left edge of the image in model space: T3(-0.01, 0.09, 0, 0){ "file://t4_image.png@0.01x0,0,0,1,0,1,0" }; // The image can also be drawn in "billboard" mode, i.e. always parallel to // the camera, by using the `#' symbol: T3(0, 0.12, 0, TextAttributes("Align", "Center")){ "file://t4_image.png@0.01x0#" }; // The size of 2D annotations is given directly in pixels: T2(350, -7, 0){ "file://t4_image.png@20x0" }; }; // This post-processing view is in the "parsed" format, i.e. it is interpreted // using the same parser as the `.geo' file. For large post-processing datasets, // that contain actual field values defined on a mesh, you should use the MSH // file format instead, which allows to efficiently store continuous or // discontinuous scalar, vector and tensor fields, or arbitrary polynomial // order. // Views and geometrical entities can be made to respond to double-click events, // here to print some messages to the console: View[0].DoubleClickedCommand = "Printf('View[0] has been double-clicked!');"; Geometry.DoubleClickedLineCommand = "Printf('Curve %g has been double-clicked!', Geometry.DoubleClickedEntityTag);"; // We can also change the color of some entities: Color Grey50{ Surface{ 22 }; } Color Purple{ Surface{ 24 }; } Color Red{ Curve{ 1:14 }; } Color Yellow{ Curve{ 15:20 }; }
Next: t6
: Transfinite meshes, Previous: t4
: Built-in functions, holes in surfaces, annotations, entity colors, Up: Tutorial [Contents][Index]
t5
: Mesh sizes, macros, loops, holes in volumesSee t5.geo. Also available in C++ (t5.cpp), Python (t5.py) and Julia (t5.jl).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 5 // // Mesh sizes, macros, loops, holes in volumes // // ----------------------------------------------------------------------------- // We start by defining some target mesh sizes: lcar1 = .1; lcar2 = .0005; lcar3 = .055; // If we wanted to change these mesh sizes globally (without changing the above // definitions), we could give a global scaling factor for all mesh sizes on the // command line with the `-clscale' option (or with `Mesh.MeshSizeFactor' in an // option file). For example, with: // // > gmsh t5.geo -clscale 1 // // this input file produces a mesh of approximately 3000 nodes and 14,000 // tetrahedra. With // // > gmsh t5.geo -clscale 0.2 // // the mesh counts approximately 231,000 nodes and 1,360,000 tetrahedra. You can // check mesh statistics in the graphical user interface with the // `Tools->Statistics' menu. // // See `t10.geo' for more information about mesh sizes. // We proceed by defining some elementary entities describing a truncated cube: Point(1) = {0.5,0.5,0.5,lcar2}; Point(2) = {0.5,0.5,0,lcar1}; Point(3) = {0,0.5,0.5,lcar1}; Point(4) = {0,0,0.5,lcar1}; Point(5) = {0.5,0,0.5,lcar1}; Point(6) = {0.5,0,0,lcar1}; Point(7) = {0,0.5,0,lcar1}; Point(8) = {0,1,0,lcar1}; Point(9) = {1,1,0,lcar1}; Point(10) = {0,0,1,lcar1}; Point(11) = {0,1,1,lcar1}; Point(12) = {1,1,1,lcar1}; Point(13) = {1,0,1,lcar1}; Point(14) = {1,0,0,lcar1}; Line(1) = {8,9}; Line(2) = {9,12}; Line(3) = {12,11}; Line(4) = {11,8}; Line(5) = {9,14}; Line(6) = {14,13}; Line(7) = {13,12}; Line(8) = {11,10}; Line(9) = {10,13}; Line(10) = {10,4}; Line(11) = {4,5}; Line(12) = {5,6}; Line(13) = {6,2}; Line(14) = {2,1}; Line(15) = {1,3}; Line(16) = {3,7}; Line(17) = {7,2}; Line(18) = {3,4}; Line(19) = {5,1}; Line(20) = {7,8}; Line(21) = {6,14}; Curve Loop(22) = {-11,-19,-15,-18}; Plane Surface(23) = {22}; Curve Loop(24) = {16,17,14,15}; Plane Surface(25) = {24}; Curve Loop(26) = {-17,20,1,5,-21,13}; Plane Surface(27) = {26}; Curve Loop(28) = {-4,-1,-2,-3}; Plane Surface(29) = {28}; Curve Loop(30) = {-7,2,-5,-6}; Plane Surface(31) = {30}; Curve Loop(32) = {6,-9,10,11,12,21}; Plane Surface(33) = {32}; Curve Loop(34) = {7,3,8,9}; Plane Surface(35) = {34}; Curve Loop(36) = {-10,18,-16,-20,4,-8}; Plane Surface(37) = {36}; Curve Loop(38) = {-14,-13,-12,19}; Plane Surface(39) = {38}; // Instead of using included files, we now use a user-defined macro in order // to carve some holes in the cube: Macro CheeseHole // In the following commands we use the reserved variable name `newp', which // automatically selects a new point tag. Analogously to `newp', the special // variables `newl', `newll, `news', `newsl' and `newv' select new curve, // curve loop, surface, surface loop and volume tags. // // If `Geometry.OldNewReg' is set to 0, the new tags are chosen as the highest // current tag for each category (points, curves, curve loops, ...), plus // one. By default, for backward compatibility, `Geometry.OldNewReg' is set // to 1, and only two categories are used: one for points and one for the // rest. p1 = newp; Point(p1) = {x, y, z, lcar3}; p2 = newp; Point(p2) = {x+r,y, z, lcar3}; p3 = newp; Point(p3) = {x, y+r,z, lcar3}; p4 = newp; Point(p4) = {x, y, z+r,lcar3}; p5 = newp; Point(p5) = {x-r,y, z, lcar3}; p6 = newp; Point(p6) = {x, y-r,z, lcar3}; p7 = newp; Point(p7) = {x, y, z-r,lcar3}; c1 = newc; Circle(c1) = {p2,p1,p7}; c2 = newc; Circle(c2) = {p7,p1,p5}; c3 = newc; Circle(c3) = {p5,p1,p4}; c4 = newc; Circle(c4) = {p4,p1,p2}; c5 = newc; Circle(c5) = {p2,p1,p3}; c6 = newc; Circle(c6) = {p3,p1,p5}; c7 = newc; Circle(c7) = {p5,p1,p6}; c8 = newc; Circle(c8) = {p6,p1,p2}; c9 = newc; Circle(c9) = {p7,p1,p3}; c10 = newc; Circle(c10) = {p3,p1,p4}; c11 = newc; Circle(c11) = {p4,p1,p6}; c12 = newc; Circle(c12) = {p6,p1,p7}; // We need non-plane surfaces to define the spherical holes. Here we use // `Surface', which can be used for surfaces with 3 or 4 curves on their // boundary. With the he built-in kernel, if the curves are circle arcs, ruled // surfaces are created; otherwise transfinite interpolation is used. // // With the OpenCASCADE kernel, `Surface' uses a much more general generic // surface filling algorithm, creating a BSpline surface passing through an // arbitrary number of boundary curves; and `ThruSections' allows to create // ruled surfaces (see `t19.geo'). l1 = newll; Curve Loop(l1) = {c5,c10,c4}; l2 = newll; Curve Loop(l2) = {c9,-c5,c1}; l3 = newll; Curve Loop(l3) = {c12,-c8,-c1}; l4 = newll; Curve Loop(l4) = {c8,-c4,c11}; l5 = newll; Curve Loop(l5) = {-c10,c6,c3}; l6 = newll; Curve Loop(l6) = {-c11,-c3,c7}; l7 = newll; Curve Loop(l7) = {-c2,-c7,-c12}; l8 = newll; Curve Loop(l8) = {-c6,-c9,c2}; s1 = news; Surface(s1) = {l1}; s2 = news; Surface(s2) = {l2}; s3 = news; Surface(s3) = {l3}; s4 = news; Surface(s4) = {l4}; s5 = news; Surface(s5) = {l5}; s6 = news; Surface(s6) = {l6}; s7 = news; Surface(s7) = {l7}; s8 = news; Surface(s8) = {l8}; // We then store the surface loops tags in a list for later reference (we will // need these to define the final volume): theloops[t] = newsl; Surface Loop(theloops[t]) = {s1, s2, s3, s4, s5, s6, s7, s8}; thehole = newv; Volume(thehole) = theloops[t]; Return // We can use a `For' loop to generate five holes in the cube: x = 0; y = 0.75; z = 0; r = 0.09; For t In {1:5} x += 0.166; z += 0.166; // We call the `CheeseHole' macro: Call CheeseHole; // We define a physical volume for each hole: Physical Volume (t) = thehole; // We also print some variables on the terminal (note that, since all // variables in `.geo' files are treated internally as floating point numbers, // the format string should only contain valid floating point format // specifiers like `%g', `%f', '%e', etc.): Printf("Hole %g (center = {%g,%g,%g}, radius = %g) has number %g!", t, x, y, z, r, thehole); EndFor // We can then define the surface loop for the exterior surface of the cube: theloops[0] = newreg; Surface Loop(theloops[0]) = {23:39:2}; // The volume of the cube, without the 5 holes, is now defined by 6 surface // loops: the first surface loop defines the exterior surface; the surface loops // other than the first one define holes. (Again, to reference an array of // variables, its identifier is followed by square brackets): Volume(186) = {theloops[]}; // Note that using solid modelling with the OpenCASCADE geometry kernel, the // same geometry could be built quite differently: see `t16.geo'. // We finally define a physical volume for the elements discretizing the cube, // without the holes (for which physical groups were already created in the // `For' loop): Physical Volume (10) = 186; // We could make only part of the model visible to only mesh this subset: // // Hide {:} // Recursive Show { Volume{129}; } // Mesh.MeshOnlyVisible=1; // Meshing algorithms can changed globally using options: Mesh.Algorithm = 6; // Frontal-Delaunay for 2D meshes // They can also be set for individual surfaces, e.g. MeshAlgorithm Surface {31, 35} = 1; // MeshAdapt on surfaces 31 and 35 // To generate a curvilinear mesh and optimize it to produce provably valid // curved elements (see A. Johnen, J.-F. Remacle and C. Geuzaine. Geometric // validity of curvilinear finite elements. Journal of Computational Physics // 233, pp. 359-372, 2013; and T. Toulorge, C. Geuzaine, J.-F. Remacle, // J. Lambrechts. Robust untangling of curvilinear meshes. Journal of // Computational Physics 254, pp. 8-26, 2013), you can uncomment the following // lines: // // Mesh.ElementOrder = 2; // Mesh.HighOrderOptimize = 2;
Next: t7
: Background meshes, Previous: t5
: Mesh sizes, macros, loops, holes in volumes, Up: Tutorial [Contents][Index]
t6
: Transfinite meshesSee t6.geo. Also available in C++ (t6.cpp) and Python (t6.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 6 // // Transfinite meshes // // ----------------------------------------------------------------------------- // Let's use the geometry from the first tutorial as a basis for this one: Include "t1.geo"; // Delete the surface and the left line, and replace the line with 3 new ones: Delete{ Surface{1}; Curve{4}; } p1 = newp; Point(p1) = {-0.05, 0.05, 0, lc}; p2 = newp; Point(p2) = {-0.05, 0.1, 0, lc}; l1 = newl; Line(l1) = {1, p1}; l2 = newl; Line(l2) = {p1, p2}; l3 = newl; Line(l3) = {p2, 4}; // Create a surface: Curve Loop(2) = {2, -1, l1, l2, l3, -3}; Plane Surface(1) = {-2}; // The `Transfinite Curve' meshing constraints explicitly specifies the location // of the nodes on the curve. For example, the following command forces 20 // uniformly placed nodes on curve 2 (including the nodes on the two end // points): Transfinite Curve{2} = 20; // Let's put 20 points total on combination of curves `l1', `l2' and `l3' // (beware that the points `p1' and `p2' are shared by the curves, so we do not // create 6 + 6 + 10 = 22 nodes, but 20!) Transfinite Curve{l1} = 6; Transfinite Curve{l2} = 6; Transfinite Curve{l3} = 10; // Finally, we put 30 nodes following a geometric progression on curve 1 // (reversed) and on curve 3: Transfinite Curve{-1, 3} = 30 Using Progression 1.2; // The `Transfinite Surface' meshing constraint uses a transfinite interpolation // algorithm in the parametric plane of the surface to connect the nodes on the // boundary using a structured grid. If the surface has more than 4 corner // points, the corners of the transfinite interpolation have to be specified by // hand: Transfinite Surface{1} = {1, 2, 3, 4}; // To create quadrangles instead of triangles, one can use the `Recombine' // command: Recombine Surface{1}; // When the surface has only 3 or 4 points on its boundary the list of corners // can be omitted in the `Transfinite Surface' constraint: Point(7) = {0.2, 0.2, 0, 1.0}; Point(8) = {0.2, 0.1, 0, 1.0}; Point(9) = {-0, 0.3, 0, 1.0}; Point(10) = {0.25, 0.2, 0, 1.0}; Point(11) = {0.3, 0.1, 0, 1.0}; Line(10) = {8, 11}; Line(11) = {11, 10}; Line(12) = {10, 7}; Line(13) = {7, 8}; Curve Loop(14) = {13, 10, 11, 12}; Plane Surface(15) = {14}; Transfinite Curve {10:13} = 10; Transfinite Surface{15}; // The way triangles are generated can be controlled by appending "Left", // "Right" or "Alternate" after the `Transfinite Surface' command. Try e.g. // // Transfinite Surface{15} Alternate; // Finally we apply an elliptic smoother to the grid to have a more regular // mesh: Mesh.Smoothing = 100;
Next: t8
: Post-processing and animations, Previous: t6
: Transfinite meshes, Up: Tutorial [Contents][Index]
t7
: Background meshesSee t7.geo. Also available in C++ (t7.cpp) and Python (t7.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 7 // // Background meshes // // ----------------------------------------------------------------------------- // Mesh sizes can be specified very accurately by providing a background mesh, // i.e., a post-processing view that contains the target mesh sizes. // Merge a list-based post-processing view containing the target mesh sizes: Merge "t7_bgmesh.pos"; // If the post-processing view was model-based instead of list-based (i.e. if it // was based on an actual mesh), we would need to create a new model to contain // the geometry so that meshing it does not destroy the background mesh. It's // not necessary here since the view is list-based, but it does no harm: NewModel; // Merge the first tutorial geometry: Merge "t1.geo"; // Apply the view as the current background mesh size field: Background Mesh View[0]; // In order to compute the mesh sizes from the background mesh only, and // disregard any other size constraints, one can set: Mesh.MeshSizeExtendFromBoundary = 0; Mesh.MeshSizeFromPoints = 0; Mesh.MeshSizeFromCurvature = 0; // See `t10.geo' for additional information: background meshes are actually a // particular case of general "mesh size fields".
Next: t9
: Plugins, Previous: t7
: Background meshes, Up: Tutorial [Contents][Index]
t8
: Post-processing and animationsSee t8.geo. Also available in C++ (t8.cpp) and Python (t8.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 8 // // Post-processing and animations // // ----------------------------------------------------------------------------- // In addition to creating geometries and meshes, GEO scripts can also be used // to manipulate post-processing datasets (called "views" in Gmsh). // We first include `t1.geo' as well as some post-processing views: Include "t1.geo"; Include "view1.pos"; Include "view1.pos"; Include "view4.pos"; // Gmsh can read post-processing views in various formats. Here the `view1.pos' // and `view4.pos' files are in the Gmsh "parsed" format, which is interpreted // directly by the GEO script parser. The parsed format should only be used for // relatively small datasets of course: for larger datasets using e.g. MSH files // is much more efficient. // We then set some general options: General.Trackball = 0; General.RotationX = 0; General.RotationY = 0; General.RotationZ = 0; General.Color.Background = White; General.Color.Foreground = Black; General.Color.Text = Black; General.Orthographic = 0; General.Axes = 0; General.SmallAxes = 0; // We also set some options for each post-processing view: v0 = PostProcessing.NbViews-4; v1 = v0+1; v2 = v0+2; v3 = v0+3; View[v0].IntervalsType = 2; View[v0].OffsetZ = 0.05; View[v0].RaiseZ = 0; View[v0].Light = 1; View[v0].ShowScale = 0; View[v0].SmoothNormals = 1; View[v1].IntervalsType = 1; View[v1].ColorTable = { Green, Blue }; View[v1].NbIso = 10; View[v1].ShowScale = 0; View[v2].Name = "Test..."; View[v2].Axes = 1; View[v2].Color.Axes = Black; View[v2].IntervalsType = 2; View[v2].Type = 2; View[v2].IntervalsType = 2; View[v2].AutoPosition = 0; View[v2].PositionX = 85; View[v2].PositionY = 50; View[v2].Width = 200; View[v2].Height = 130; View[v3].Visible = 0; // You can save an MPEG movie directly by selecting `File->Export' in the // GUI. Several predefined animations are setup, for looping on all the time // steps in views, or for looping between views. // But a script can be used to build much more complex animations, by changing // options at run-time and re-rendering the graphics. Each frame can then be // saved to disk as an image, and multiple frames can be encoded to form a // movie. Below is an example of such a custom animation. t = 0; // Initial step // Loop on num from 1 to 3 For num In {1:3} View[v0].TimeStep = t; // Set time step View[v1].TimeStep = t; View[v2].TimeStep = t; View[v3].TimeStep = t; t = (View[v0].TimeStep < View[v0].NbTimeStep-1) ? t+1 : 0; // Increment View[v0].RaiseZ += 0.01/View[v0].Max * t; // Raise view v0 If (num == 3) // Resize the graphics when num == 3, to create 640x480 frames General.GraphicsWidth = General.MenuWidth + 640; General.GraphicsHeight = 480; EndIf frames = 50; // Loop on num2 from 1 to frames For num2 In {1:frames} // Incrementally rotate the scene General.RotationX += 10; General.RotationY = General.RotationX / 3; General.RotationZ += 0.1; // Sleep for 0.01 second Sleep 0.01; // Draw the scene (one could use `DrawForceChanged' instead to force the // reconstruction of the vertex arrays, e.g. if changing element clipping) Draw; If (num == 3) // Uncomment the following lines to save each frame to an image file (the // `Print' command saves the graphical window; the `Sprintf' function // permits to create the file names on the fly): // Print Sprintf("t8-%02g.gif", num2); // Print Sprintf("t8-%02g.ppm", num2); // Print Sprintf("t8-%02g.jpg", num2); EndIf EndFor If(num == 3) // Here we could make a system call to generate a movie. For example, // with whirlgif: /* System "whirlgif -minimize -loop -o t8.gif t8-*.gif"; */ // with mpeg_encode (create parameter file first, then run encoder): /* Printf("PATTERN I") > "t8.par"; Printf("BASE_FILE_FORMAT PPM") >> "t8.par"; Printf("GOP_SIZE 1") >> "t8.par"; Printf("SLICES_PER_FRAME 1") >> "t8.par"; Printf("PIXEL HALF") >> "t8.par"; Printf("RANGE 10") >> "t8.par"; Printf("PSEARCH_ALG EXHAUSTIVE") >> "t8.par"; Printf("BSEARCH_ALG CROSS2") >> "t8.par"; Printf("IQSCALE 1") >> "t8.par"; Printf("PQSCALE 1") >> "t8.par"; Printf("BQSCALE 25") >> "t8.par"; Printf("REFERENCE_FRAME DECODED") >> "t8.par"; Printf("OUTPUT t8.mpg") >> "t8.par"; Printf("INPUT_CONVERT *") >> "t8.par"; Printf("INPUT_DIR .") >> "t8.par"; Printf("INPUT") >> "t8.par"; tmp = Sprintf("t8-*.ppm [01-%02g]", frames); Printf(tmp) >> "t8.par"; Printf("END_INPUT") >> "t8.par"; System "mpeg_encode t8.par"; */ // with mencoder: /* System "mencoder 'mf://*.jpg' -mf fps=5 -o t8.mpg -ovc lavc -lavcopts vcodec=mpeg1video:vhq"; System "mencoder 'mf://*.jpg' -mf fps=5 -o t8.mpg -ovc lavc -lavcopts vcodec=mpeg4:vhq"; */ // with ffmpeg: /* System "ffmpeg -hq -r 5 -b 800 -vcodec mpeg1video -i t8-%02d.jpg t8.mpg" System "ffmpeg -hq -r 5 -b 800 -i t8-%02d.jpg t8.asf" */ EndIf EndFor
Next: t10
: Mesh size fields, Previous: t8
: Post-processing and animations, Up: Tutorial [Contents][Index]
t9
: PluginsSee t9.geo. Also available in C++ (t9.cpp) and Python (t9.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 9 // // Plugins // // ----------------------------------------------------------------------------- // Plugins can be added to Gmsh in order to extend its capabilities. For // example, post-processing plugins can modify views, or create new views based // on previously loaded views. Several default plugins are statically linked // with Gmsh, e.g. Isosurface, CutPlane, CutSphere, Skin, Transform or Smooth. // // Plugins can be controlled in the same way as other options: either from the // graphical interface (right click on the view button, then `Plugins'), or from // the command file. // Let us for example include a three-dimensional scalar view: Include "view3.pos" ; // We then set some options for the `Isosurface' plugin (which extracts an // isosurface from a 3D scalar view), and run it: Plugin(Isosurface).Value = 0.67 ; // Iso-value level Plugin(Isosurface).View = 0 ; // Source view is View[0] Plugin(Isosurface).Run ; // Run the plugin! // We also set some options for the `CutPlane' plugin (which computes a section // of a 3D view using the plane A*x+B*y+C*z+D=0), and then run it: Plugin(CutPlane).A = 0 ; Plugin(CutPlane).B = 0.2 ; Plugin(CutPlane).C = 1 ; Plugin(CutPlane).D = 0 ; Plugin(CutPlane).View = 0 ; Plugin(CutPlane).Run ; // Add a title (By convention, for window coordinates a value greater than 99999 // represents the center. We could also use `General.GraphicsWidth / 2', but // that would only center the string for the current window size.): Plugin(Annotate).Text = "A nice title" ; Plugin(Annotate).X = 1.e5; Plugin(Annotate).Y = 50 ; Plugin(Annotate).Font = "Times-BoldItalic" ; Plugin(Annotate).FontSize = 28 ; Plugin(Annotate).Align = "Center" ; Plugin(Annotate).View = 0 ; Plugin(Annotate).Run ; Plugin(Annotate).Text = "(and a small subtitle)" ; Plugin(Annotate).Y = 70 ; Plugin(Annotate).Font = "Times-Roman" ; Plugin(Annotate).FontSize = 12 ; Plugin(Annotate).Run ; // We finish by setting some options: View[0].Light = 1; View[0].IntervalsType = 1; View[0].NbIso = 6; View[0].SmoothNormals = 1; View[1].IntervalsType = 2; View[2].IntervalsType = 2;
Next: t11
: Unstructured quadrangular meshes, Previous: t9
: Plugins, Up: Tutorial [Contents][Index]
t10
: Mesh size fieldsSee t10.geo. Also available in C++ (t10.cpp) and Python (t10.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 10 // // Mesh size fields // // ----------------------------------------------------------------------------- // In addition to specifying target mesh sizes at the points of the geometry // (see `t1.geo') or using a background mesh (see `t7.geo'), you can use general // mesh size "Fields". // Let's create a simple rectangular geometry lc = .15; Point(1) = {0.0,0.0,0,lc}; Point(2) = {1,0.0,0,lc}; Point(3) = {1,1,0,lc}; Point(4) = {0,1,0,lc}; Point(5) = {0.2,.5,0,lc}; Line(1) = {1,2}; Line(2) = {2,3}; Line(3) = {3,4}; Line(4) = {4,1}; Curve Loop(5) = {1,2,3,4}; Plane Surface(6) = {5}; // Say we would like to obtain mesh elements with size lc/30 near curve 2 and // point 5, and size lc elsewhere. To achieve this, we can use two fields: // "Distance", and "Threshold". We first define a Distance field (`Field[1]') on // points 5 and on curve 2. This field returns the distance to point 5 and to // (100 equidistant points on) curve 2. Field[1] = Distance; Field[1].PointsList = {5}; Field[1].CurvesList = {2}; Field[1].NumPointsPerCurve = 100; // We then define a `Threshold' field, which uses the return value of the // `Distance' field 1 in order to define a simple change in element size // depending on the computed distances // // SizeMax - /------------------ // / // / // / // SizeMin -o----------------/ // | | | // Point DistMin DistMax Field[2] = Threshold; Field[2].InField = 1; Field[2].SizeMin = lc / 30; Field[2].SizeMax = lc; Field[2].DistMin = 0.15; Field[2].DistMax = 0.5; // Say we want to modulate the mesh element sizes using a mathematical function // of the spatial coordinates. We can do this with the MathEval field: Field[3] = MathEval; Field[3].F = "Cos(4*3.14*x) * Sin(4*3.14*y) / 10 + 0.101"; // We could also combine MathEval with values coming from other fields. For // example, let's define a `Distance' field around point 1 Field[4] = Distance; Field[4].PointsList = {1}; // We can then create a `MathEval' field with a function that depends on the // return value of the `Distance' field 4, i.e., depending on the distance to // point 1 (here using a cubic law, with minimum element size = lc / 100) Field[5] = MathEval; Field[5].F = Sprintf("F4^3 + %g", lc / 100); // We could also use a `Box' field to impose a step change in element sizes // inside a box Field[6] = Box; Field[6].VIn = lc / 15; Field[6].VOut = lc; Field[6].XMin = 0.3; Field[6].XMax = 0.6; Field[6].YMin = 0.3; Field[6].YMax = 0.6; // Many other types of fields are available: see the reference manual for a // complete list. You can also create fields directly in the graphical user // interface by selecting `Define->Size fields' in the `Mesh' module. // Finally, let's use the minimum of all the fields as the background mesh size // field Field[7] = Min; Field[7].FieldsList = {2, 3, 5, 6}; Background Field = 7; // To determine the size of mesh elements, Gmsh locally computes the minimum of // // 1) the size of the model bounding box; // 2) if `Mesh.MeshSizeFromPoints' is set, the mesh size specified at // geometrical points; // 3) if `Mesh.MeshSizeFromCurvature' is positive, the mesh size based on // curvature (the value specifying the number of elements per 2 * pi rad); // 4) the background mesh size field; // 5) any per-entity mesh size constraint. // // This value is then constrained in the interval [`Mesh.MeshSizeMin', // `Mesh.MeshSizeMax'] and multiplied by `Mesh.MeshSizeFactor'. In addition, // boundary mesh sizes (on curves or surfaces) are interpolated inside the // enclosed entity (surface or volume, respectively) if the option // `Mesh.MeshSizeExtendFromBoundary' is set (which is the case by default). // // When the element size is fully specified by a background mesh size field (as // it is in this example), it is thus often desirable to set Mesh.MeshSizeExtendFromBoundary = 0; Mesh.MeshSizeFromPoints = 0; Mesh.MeshSizeFromCurvature = 0; // This will prevent over-refinement due to small mesh sizes on the boundary.
Next: t12
: Cross-patch meshing with compounds, Previous: t10
: Mesh size fields, Up: Tutorial [Contents][Index]
t11
: Unstructured quadrangular meshesSee t11.geo. Also available in C++ (t11.cpp) and Python (t11.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 11 // // Unstructured quadrangular meshes // // ----------------------------------------------------------------------------- // We have seen in tutorials `t3.geo' and `t6.geo' that extruded and transfinite // meshes can be "recombined" into quads, prisms or hexahedra by using the // "Recombine" keyword. Unstructured meshes can be recombined in the same // way. Let's define a simple geometry with an analytical mesh size field: Point(1) = {-1.25, -.5, 0}; Point(2) = {1.25, -.5, 0}; Point(3) = {1.25, 1.25, 0}; Point(4) = {-1.25, 1.25, 0}; Line(1) = {1, 2}; Line(2) = {2, 3}; Line(3) = {3, 4}; Line(4) = {4, 1}; Curve Loop(4) = {1, 2, 3, 4}; Plane Surface(100) = {4}; Field[1] = MathEval; Field[1].F = "0.01*(1.0+30.*(y-x*x)*(y-x*x) + (1-x)*(1-x))"; Background Field = 1; // To generate quadrangles instead of triangles, we can simply add Recombine Surface{100}; // If we'd had several surfaces, we could have used `Recombine Surface {:};'. // Yet another way would be to specify the global option "Mesh.RecombineAll = // 1;". // The default recombination algorithm is called "Blossom": it uses a minimum // cost perfect matching algorithm to generate fully quadrilateral meshes from // triangulations. More details about the algorithm can be found in the // following paper: J.-F. Remacle, J. Lambrechts, B. Seny, E. Marchandise, // A. Johnen and C. Geuzaine, "Blossom-Quad: a non-uniform quadrilateral mesh // generator using a minimum cost perfect matching algorithm", International // Journal for Numerical Methods in Engineering 89, pp. 1102-1119, 2012. // For even better 2D (planar) quadrilateral meshes, you can try the // experimental "Frontal-Delaunay for quads" meshing algorithm, which is a // triangulation algorithm that enables to create right triangles almost // everywhere: J.-F. Remacle, F. Henrotte, T. Carrier-Baudouin, E. Bechet, // E. Marchandise, C. Geuzaine and T. Mouton. A frontal Delaunay quad mesh // generator using the L^inf norm. International Journal for Numerical Methods // in Engineering, 94, pp. 494-512, 2013. Uncomment the following line to try // the Frontal-Delaunay algorithms for quads: // // Mesh.Algorithm = 8; // The default recombination algorithm might leave some triangles in the mesh, // if recombining all the triangles leads to badly shaped quads. In such cases, // to generate full-quad meshes, you can either subdivide the resulting hybrid // mesh (with Mesh.SubdivisionAlgorithm = 1), or use the full-quad recombination // algorithm, which will automatically perform a coarser mesh followed by // recombination, smoothing and subdivision. Uncomment the following line to try // the full-quad algorithm: // // Mesh.RecombinationAlgorithm = 2; // or 3 // Note that you could also apply the recombination algorithm and/or the // subdivision step explicitly after meshing, as follows: // // Mesh 2; // RecombineMesh; // Mesh.SubdivisionAlgorithm = 1; // RefineMesh;
Next: t13
: Remeshing an STL file without an underlying CAD model, Previous: t11
: Unstructured quadrangular meshes, Up: Tutorial [Contents][Index]
t12
: Cross-patch meshing with compoundsSee t12.geo/ Also available in C++ (t12.cpp) and Python (t12.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 12 // // Cross-patch meshing with compounds // // ----------------------------------------------------------------------------- // "Compound" meshing constraints allow to generate meshes across surface // boundaries, which can be useful e.g. for imported CAD models (e.g. STEP) with // undesired small features. // When a `Compound Curve' or `Compound Surface' meshing constraint is given, // at mesh generation time Gmsh // 1. meshes the underlying elementary geometrical entities, individually // 2. creates a discrete entity that combines all the individual meshes // 3. computes a discrete parametrization (i.e. a piece-wise linear mapping) // on this discrete entity // 4. meshes the discrete entity using this discrete parametrization instead // of the underlying geometrical description of the underlying elementary // entities making up the compound // 5. optionally, reclassifies the mesh elements and nodes on the original // entities // Step 3. above can only be performed if the mesh resulting from the // combination of the individual meshes can be reparametrized, i.e. if the shape // is "simple enough". If the shape is not amenable to reparametrization, you // should create a full mesh of the geometry and first re-classify it to // generate patches amenable to reparametrization (see `t13.geo'). // The mesh of the individual entities performed in Step 1. should usually be // finer than the desired final mesh; this can be controlled with the // `Mesh.CompoundMeshSizeFactor' option. // The optional reclassification on the underlying elementary entities in Step // 5. is governed by the `Mesh.CompoundClassify' option. lc = 0.1; Point(1) = {0, 0, 0, lc}; Point(2) = {1, 0, 0, lc}; Point(3) = {1, 1, 0.5, lc}; Point(4) = {0, 1, 0.4, lc}; Point(5) = {0.3, 0.2, 0, lc}; Point(6) = {0, 0.01, 0.01, lc}; Point(7) = {0, 0.02, 0.02, lc}; Point(8) = {1, 0.05, 0.02, lc}; Point(9) = {1, 0.32, 0.02, lc}; Line(1) = {1, 2}; Line(2) = {2, 8}; Line(3) = {8, 9}; Line(4) = {9, 3}; Line(5) = {3, 4}; Line(6) = {4, 7}; Line(7) = {7, 6}; Line(8) = {6, 1}; Spline(9) = {7, 5, 9}; Line(10) = {6, 8}; Curve Loop(11) = {5, 6, 9, 4}; Surface(1) = {11}; Curve Loop(13) = {-9, 3, 10, 7}; Surface(5) = {13}; Curve Loop(15) = {-10, 2, 1, 8}; Surface(10) = {15}; // Treat curves 2, 3 and 4 as a single curve when meshing (i.e. mesh across // points 6 and 7) Compound Curve{2, 3, 4}; // Idem with curves 6, 7 and 8 Compound Curve{6, 7, 8}; // Treat surfaces 1, 5 and 10 as a single surface when meshing (i.e. mesh across // curves 9 and 10) Compound Surface{1, 5, 10};
Next: t14
: Homology and cohomology computation, Previous: t12
: Cross-patch meshing with compounds, Up: Tutorial [Contents][Index]
t13
: Remeshing an STL file without an underlying CAD modelSee t13.geo. Also available in C++ (t13.cpp) and Python (t13.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 13 // // Remeshing an STL file without an underlying CAD model // // ----------------------------------------------------------------------------- // Let's merge an STL mesh that we would like to remesh. Merge "t13_data.stl"; // We first classify ("color") the surfaces by splitting the original surface // along sharp geometrical features. This will create new discrete surfaces, // curves and points. DefineConstant[ // Angle between two triangles above which an edge is considered as sharp angle = {40, Min 20, Max 120, Step 1, Name "Parameters/Angle for surface detection"}, // For complex geometries, patches can be too complex, too elongated or too // large to be parametrized; setting the following option will force the // creation of patches that are amenable to reparametrization: forceParametrizablePatches = {0, Choices{0,1}, Name "Parameters/Create surfaces guaranteed to be parametrizable"}, // For open surfaces include the boundary edges in the classification process: includeBoundary = 1, // Force curves to be split on given angle: curveAngle = 180 ]; ClassifySurfaces{angle * Pi/180, includeBoundary, forceParametrizablePatches, curveAngle * Pi / 180}; // Create a geometry for all the discrete curves and surfaces in the mesh, by // computing a parametrization for each one CreateGeometry; // In batch mode the two steps above can be performed with `gmsh t13.stl // -reparam 40', which will save `t13.msh' containing the parametrizations, and // which can thus subsequently be remeshed. // Note that if a CAD model (e.g. as a STEP file, see `t20.geo') is available // instead of an STL mesh, it is usually better to use that CAD model instead of // the geometry created by reparametrizing the mesh. Indeed, CAD geometries will // in general be more accurate, with smoother parametrizations, and will lead to // more efficient and higher quality meshing. Discrete surface remeshing in Gmsh // is optimized to handle dense STL meshes coming from e.g. imaging systems // where no CAD is available; it is less well suited for the poor quality STL // triangulations (optimized for size, with e.g. very elongated triangles) that // are usually generated by CAD tools for e.g. 3D printing. // Create a volume as usual Surface Loop(1) = Surface{:}; Volume(1) = {1}; // We specify element sizes imposed by a size field, just because we can :-) funny = DefineNumber[0, Choices{0,1}, Name "Parameters/Apply funny mesh size field?" ]; Field[1] = MathEval; If(funny) Field[1].F = "2*Sin((x+y)/5) + 3"; Else Field[1].F = "4"; EndIf Background Field = 1;
Next: t15
: Embedded points, lines and surfaces, Previous: t13
: Remeshing an STL file without an underlying CAD model, Up: Tutorial [Contents][Index]
t14
: Homology and cohomology computationSee t14.geo. Also available in C++ (t14.cpp) and Python (t14.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 14 // // Homology and cohomology computation // // ----------------------------------------------------------------------------- // Homology computation in Gmsh finds representative chains of (relative) // (co)homology space bases using a mesh of a model. The representative basis // chains are stored in the mesh as physical groups of Gmsh, one for each chain. // Create an example geometry m = 0.5; // mesh size h = 2; // height in the z-direction Point(1) = {0, 0, 0, m}; Point(2) = {10, 0, 0, m}; Point(3) = {10, 10, 0, m}; Point(4) = {0, 10, 0, m}; Point(5) = {4, 4, 0, m}; Point(6) = {6, 4, 0, m}; Point(7) = {6, 6, 0, m}; Point(8) = {4, 6, 0, m}; Point(9) = {2, 0, 0, m}; Point(10) = {8, 0, 0, m}; Point(11) = {2, 10, 0, m}; Point(12) = {8, 10, 0, m}; Line(1) = {1, 9}; Line(2) = {9, 10}; Line(3) = {10, 2}; Line(4) = {2, 3}; Line(5) = {3, 12}; Line(6) = {12, 11}; Line(7) = {11, 4}; Line(8) = {4, 1}; Line(9) = {5, 6}; Line(10) = {6, 7}; Line(11) = {7, 8}; Line(12) = {8, 5}; Curve Loop(13) = {6, 7, 8, 1, 2, 3, 4, 5}; Curve Loop(14) = {11, 12, 9, 10}; Plane Surface(15) = {13, 14}; e() = Extrude {0, 0, h}{ Surface{15}; }; // Create physical groups, which are used to define the domain of the // (co)homology computation and the subdomain of the relative (co)homology // computation. // Whole domain Physical Volume(1) = {e(1)}; // Four "terminals" of the model Physical Surface(70) = {e(3)}; Physical Surface(71) = {e(5)}; Physical Surface(72) = {e(7)}; Physical Surface(73) = {e(9)}; // Whole domain surface bnd() = Boundary{ Volume{e(1)}; }; Physical Surface(80) = bnd(); // Complement of the domain surface with respect to the four terminals bnd() -= {e(3), e(5), e(7), e(9)}; Physical Surface(75) = bnd(); // Find bases for relative homology spaces of the domain modulo the four // terminals. Homology {{1}, {70, 71, 72, 73}}; // Find homology space bases isomorphic to the previous bases: homology spaces // modulo the non-terminal domain surface, a.k.a the thin cuts. Homology {{1}, {75}}; // Find cohomology space bases isomorphic to the previous bases: cohomology // spaces of the domain modulo the four terminals, a.k.a the thick cuts. Cohomology {{1}, {70, 71, 72, 73}}; // More examples: // Homology {1}; // Homology; // Homology {{1}, {80}}; // Homology {{}, {80}}; // For more information, see M. Pellikka, S. Suuriniemi, L. Kettunen and // C. Geuzaine. Homology and cohomology computation in finite element // modeling. SIAM Journal on Scientific Computing 35(5), pp. 1195-1214, 2013.
Next: t16
: Constructive Solid Geometry, OpenCASCADE geometry kernel, Previous: t14
: Homology and cohomology computation, Up: Tutorial [Contents][Index]
t15
: Embedded points, lines and surfacesSee t15.geo. Also available in C++ (t15.cpp) and Python (t15.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 15 // // Embedded points, lines and surfaces // // ----------------------------------------------------------------------------- // By default, across geometrical dimensions meshes generated by Gmsh are only // conformal if lower dimensional entities are on the boundary of higher // dimensional ones (i.e. if points, curves or surfaces are part of the boundary // of volumes). // Embedding constraints allow to force a mesh to be conformal to other lower // dimensional entities. // We start one again by including the first tutorial: Include "t1.geo"; // We change the mesh size to generate coarser mesh lc = lc * 4; MeshSize {1:4} = lc; // We define a new point Point(5) = {0.02, 0.02, 0, lc}; // One can force this point to be included ("embedded") in the 2D mesh, using // the `Point In Surface' command: Point{5} In Surface{1}; // In the same way, one can force a curve to be embedded in the 2D mesh using // the `Curve in Surface' command: Point(6) = {0.02, 0.12, 0, lc}; Point(7) = {0.04, 0.18, 0, lc}; Line(5) = {6, 7}; Curve{5} In Surface{1}; // One can also embed points and curves in a volume using the `Curve/Point In // Volume' commands: Extrude {0, 0, 0.1}{ Surface {1}; } p = newp; Point(p) = {0.07, 0.15, 0.025, lc}; Point{p} In Volume {1}; l = newl; Point(p+1) = {0.025, 0.15, 0.025, lc}; Line(l) = {7, p+1}; Curve{l} In Volume {1}; // Finally, one can also embed a surface in a volume using the `Surface In // Volume' command: Point(p+2) = {0.02, 0.12, 0.05, lc}; Point(p+3) = {0.04, 0.12, 0.05, lc}; Point(p+4) = {0.04, 0.18, 0.05, lc}; Point(p+5) = {0.02, 0.18, 0.05, lc}; Line(l+1) = {p+2, p+3}; Line(l+2) = {p+3, p+4}; Line(l+3) = {p+4, p+5}; Line(l+4) = {p+5, p+2}; ll = newll; Curve Loop(ll) = {l+1:l+4}; s = news; Plane Surface(s) = {ll}; Surface{s} In Volume {1}; // Note that with the OpenCASCADE kernel (see `t16.geo'), when the // `BooleanFragments' command is applied to entities of different dimensions, // the lower dimensional entities will be autmatically embedded in the higher // dimensional entities if necessary. Physical Point("Embedded point") = {p}; Physical Curve("Embdded curve") = {l}; Physical Surface("Embedded surface") = {s}; Physical Volume("Volume") = {1};
Next: t17
: Anisotropic background mesh, Previous: t15
: Embedded points, lines and surfaces, Up: Tutorial [Contents][Index]
t16
: Constructive Solid Geometry, OpenCASCADE geometry kernelSee t16.geo. Also available in C++ (t16.cpp), Python (t16.py) and Julia (t16.jl).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 16 // // Constructive Solid Geometry, OpenCASCADE geometry kernel // // ----------------------------------------------------------------------------- // Instead of constructing a model in a bottom-up fashion with Gmsh's built-in // geometry kernel, starting with version 3 Gmsh allows you to directly use // alternative geometry kernels. Here we use the OpenCASCADE kernel: SetFactory("OpenCASCADE"); // Let's build the same model as in `t5.geo', but using constructive solid // geometry. // We first create two cubes: Box(1) = {0,0,0, 1,1,1}; Box(2) = {0,0,0, 0.5,0.5,0.5}; // We apply a boolean difference to create the "cube minus one eigth" shape: BooleanDifference(3) = { Volume{1}; Delete; }{ Volume{2}; Delete; }; // Boolean operations with OpenCASCADE always create new entities. Adding // `Delete' in the arguments allows to automatically delete the original // entities. // We then create the five spheres: x = 0 ; y = 0.75 ; z = 0 ; r = 0.09 ; For t In {1:5} x += 0.166 ; z += 0.166 ; Sphere(3 + t) = {x,y,z,r}; Physical Volume(t) = {3 + t}; EndFor // If we had wanted five empty holes we would have used `BooleanDifference' // again. Here we want five spherical inclusions, whose mesh should be conformal // with the mesh of the cube: we thus use `BooleanFragments', which intersects // all volumes in a conformal manner (without creating duplicate interfaces): v() = BooleanFragments{ Volume{3}; Delete; }{ Volume{3 + 1 : 3 + 5}; Delete; }; // When the boolean operation leads to simple modifications of entities, and if // one deletes the original entities with `Delete', Gmsh tries to assign the // same tag to the new entities. (This behavior is governed by the // `Geometry.OCCBooleanPreserveNumbering' option.) // Here the `Physical Volume' definitions made above will thus still work, as // the five spheres (volumes 4, 5, 6, 7 and 8), which will be deleted by the // fragment operations, will be recreated identically (albeit with new surfaces) // with the same tags. // The tag of the cube will change though, so we need to access it // programmatically: Physical Volume(10) = v(#v()-1); // Creating entities using constructive solid geometry is very powerful, but can // lead to practical issues for e.g. setting mesh sizes at points, or // identifying boundaries. // To identify points or other bounding entities you can take advantage of the // `PointfsOf' (a special case of the more general `Boundary' command) and the // `In BoundingBox' commands. lcar1 = .1; lcar2 = .0005; lcar3 = .055; eps = 1e-3; // Assign a mesh size to all the points of all the volumes: MeshSize{ PointsOf{ Volume{:}; } } = lcar1; // Override this constraint on the points of the five spheres: MeshSize{ PointsOf{ Volume{3 + 1 : 3 + 5}; } } = lcar3; // Select the corner point by searching for it geometrically: p() = Point In BoundingBox{0.5-eps, 0.5-eps, 0.5-eps, 0.5+eps, 0.5+eps, 0.5+eps}; MeshSize{ p() } = lcar2; // Additional examples created with the OpenCASCADE geometry kernel are // available in `t18.geo', `t19.geo' and `t20.geo', as well as in the // `demos/boolean' directory.
Next: t18
: Periodic meshes, Previous: t16
: Constructive Solid Geometry, OpenCASCADE geometry kernel, Up: Tutorial [Contents][Index]
t17
: Anisotropic background meshSee t17.geo. Also available in C++ (t17.cpp) and Python (t17.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 17 // // Anisotropic background mesh // // ----------------------------------------------------------------------------- // As seen in `t7.geo', mesh sizes can be specified very accurately by providing // a background mesh, i.e., a post-processing view that contains the target mesh // sizes. // Here, the background mesh is represented as a metric tensor field defined on // a square. One should use bamg as 2d mesh generator to enable anisotropic // meshes in 2D. SetFactory("OpenCASCADE"); // Create a square Rectangle(1) = {-1, -1, 0, 2, 2}; // Merge a post-processing view containing the target anisotropic mesh sizes Merge "t17_bgmesh.pos"; // Apply the view as the current background mesh Background Mesh View[0]; // Use bamg Mesh.SmoothRatio = 3; Mesh.AnisoMax = 1000; Mesh.Algorithm = 7;
Next: t19
: Thrusections, fillets, pipes, mesh size from curvature, Previous: t17
: Anisotropic background mesh, Up: Tutorial [Contents][Index]
t18
: Periodic meshesSee t18.geo. Also available in C++ (t18.cpp) and Python (t18.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 18 // // Periodic meshes // // ----------------------------------------------------------------------------- // Periodic meshing constraints can be imposed on surfaces and curves. // Let's use the OpenCASCADE geometry kernel to build two geometries. SetFactory("OpenCASCADE"); // The first geometry is very simple: a unit cube with a non-uniform mesh size // constraint (set on purpose to be able to verify visually that the periodicity // constraint works!): Box(1) = {0, 0, 0, 1, 1, 1}; MeshSize {:} = 0.1; MeshSize {1} = 0.02; // To impose that the mesh on surface 2 (the right side of the cube) should // match the mesh from surface 1 (the left side), the following periodicity // constraint is set: Periodic Surface {2} = {1} Translate {1, 0, 0}; // During mesh generation, the mesh on surface 2 will be created by copying the // mesh from surface 1. Periodicity constraints can be specified with a // `Translation', a `Rotation' or a general `Affine' transform. // Multiple periodicities can be imposed in the same way: Periodic Surface {6} = {5} Translate {0, 0, 1}; Periodic Surface {4} = {3} Translate {0, 1, 0}; // For more complicated cases, finding the corresponding surfaces by hand can be // tedious, especially when geometries are created through solid // modelling. Let's construct a slightly more complicated geometry. // We start with a cube and some spheres: Box(10) = {2, 0, 0, 1, 1, 1}; x = 2-0.3; y = 0; z = 0; Sphere(11) = {x, y, z, 0.35}; Sphere(12) = {x+1, y, z, 0.35}; Sphere(13) = {x, y+1, z, 0.35}; Sphere(14) = {x, y, z+1, 0.35}; Sphere(15) = {x+1, y+1, z, 0.35}; Sphere(16) = {x, y+1, z+1, 0.35}; Sphere(17) = {x+1, y, z+1, 0.35}; Sphere(18) = {x+1, y+1, z+1, 0.35}; // We first fragment all the volumes, which will leave parts of spheres // protruding outside the cube: v() = BooleanFragments { Volume{10}; Delete; }{ Volume{11:18}; Delete; }; // Ask OpenCASCADE to compute more accurate bounding boxes of entities using the // STL mesh: Geometry.OCCBoundsUseStl = 1; // We then retrieve all the volumes in the bounding box of the original cube, // and delete all the parts outside it: eps = 1e-3; vin() = Volume In BoundingBox {2-eps,-eps,-eps, 2+1+eps,1+eps,1+eps}; v() -= vin(); Recursive Delete{ Volume{v()}; } // We now set a non-uniform mesh size constraint (again to check results // visually): MeshSize { PointsOf{ Volume{vin()}; }} = 0.1; p() = Point In BoundingBox{2-eps, -eps, -eps, 2+eps, eps, eps}; MeshSize {p()} = 0.001; // We now identify corresponding surfaces on the left and right sides of the // geometry automatically. // First we get all surfaces on the left: Sxmin() = Surface In BoundingBox{2-eps, -eps, -eps, 2+eps, 1+eps, 1+eps}; For i In {0:#Sxmin()-1} // Then we get the bounding box of each left surface bb() = BoundingBox Surface { Sxmin(i) }; // We translate the bounding box to the right and look for surfaces inside it: Sxmax() = Surface In BoundingBox { bb(0)-eps+1, bb(1)-eps, bb(2)-eps, bb(3)+eps+1, bb(4)+eps, bb(5)+eps }; // For all the matches, we compare the corresponding bounding boxes... For j In {0:#Sxmax()-1} bb2() = BoundingBox Surface { Sxmax(j) }; bb2(0) -= 1; bb2(3) -= 1; // ...and if they match, we apply the periodicity constraint If(Fabs(bb2(0)-bb(0)) < eps && Fabs(bb2(1)-bb(1)) < eps && Fabs(bb2(2)-bb(2)) < eps && Fabs(bb2(3)-bb(3)) < eps && Fabs(bb2(4)-bb(4)) < eps && Fabs(bb2(5)-bb(5)) < eps) Periodic Surface {Sxmax(j)} = {Sxmin(i)} Translate {1,0,0}; EndIf EndFor EndFor
Next: t20
: STEP import and manipulation, geometry partitioning, Previous: t18
: Periodic meshes, Up: Tutorial [Contents][Index]
t19
: Thrusections, fillets, pipes, mesh size from curvatureSee t19.geo. Also available in C++ (t19.cpp) and Python (t19.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 19 // // Thrusections, fillets, pipes, mesh size from curvature // // ----------------------------------------------------------------------------- // The OpenCASCADE geometry kernel supports several useful features for solid // modelling. SetFactory("OpenCASCADE"); // Volumes can be constructed from (closed) curve loops thanks to the // `ThruSections' command Circle(1) = {0,0,0, 0.5}; Curve Loop(1) = 1; Circle(2) = {0.1,0.05,1, 0.1}; Curve Loop(2) = 2; Circle(3) = {-0.1,-0.1,2, 0.3}; Curve Loop(3) = 3; ThruSections(1) = {1:3}; // With `Ruled ThruSections' you can force the use of ruled surfaces: Circle(11) = {2+0,0,0, 0.5}; Curve Loop(11) = 11; Circle(12) = {2+0.1,0.05,1, 0.1}; Curve Loop(12) = 12; Circle(13) = {2-0.1,-0.1,2, 0.3}; Curve Loop(13) = 13; Ruled ThruSections(11) = {11:13}; // We copy the first volume, and fillet all its edges: v() = Translate{4, 0, 0} { Duplicata{ Volume{1}; } }; f() = Abs(Boundary{ Volume{v(0)}; }); e() = Unique(Abs(Boundary{ Surface{f()}; })); Fillet{v(0)}{e()}{0.1} // OpenCASCADE also allows general extrusions along a smooth path. Let's first // define a spline curve: nturns = 1; npts = 20; r = 1; h = 1 * nturns; For i In {0 : npts - 1} theta = i * 2*Pi*nturns/npts; Point(1000 + i) = {r * Cos(theta), r * Sin(theta), i * h/npts}; EndFor Spline(1000) = {1000 : 1000 + npts - 1}; // A wire is like a curve loop, but open: Wire(1000) = {1000}; // We define the shape we would like to extrude along the spline (a disk): Disk(1000) = {1,0,0, 0.2}; Rotate {{1, 0, 0}, {0, 0, 0}, Pi/2} { Surface{1000}; } // We extrude the disk along the spline to create a pipe: Extrude { Surface{1000}; } Using Wire {1000} // We delete the source surface, and increase the number of sub-edges for a // nicer display of the geometry: Delete{ Surface{1000}; } Geometry.NumSubEdges = 1000; // We can activate the calculation of mesh element sizes based on curvature // (here with a target of 20 elements per 2*Pi radians): Mesh.MeshSizeFromCurvature = 20; // We can constraint the min and max element sizes to stay within reasonnable // values (see `t10.geo' for more details): Mesh.MeshSizeMin = 0.001; Mesh.MeshSizeMax = 0.3;
Next: t21
: Mesh partitioning, Previous: t19
: Thrusections, fillets, pipes, mesh size from curvature, Up: Tutorial [Contents][Index]
t20
: STEP import and manipulation, geometry partitioningSee t20.geo. Also available in C++ (t20.cpp) and Python (t20.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 20 // // STEP import and manipulation, geometry partitioning // // ----------------------------------------------------------------------------- // The OpenCASCADE geometry kernel allows to import STEP files and to modify // them. In this tutorial we will load a STEP geometry and partition it into // slices. SetFactory("OpenCASCADE"); // Load a STEP file (using `ShapeFromFile' instead of `Merge' allows to directly // retrieve the tags of the highest dimensional imported entities): v() = ShapeFromFile("t20_data.step"); // If we had specified // // Geometry.OCCTargetUnit = "M"; // // before merging the STEP file, OpenCASCADE would have converted the units to // meters (instead of the default, which is millimeters). // Get the bounding box of the volume: bbox() = BoundingBox Volume{v()}; xmin = bbox(0); ymin = bbox(1); zmin = bbox(2); xmax = bbox(3); ymax = bbox(4); zmax = bbox(5); // We want to slice the model into N slices, and either keep the volume slices // or just the surfaces obtained by the cutting: DefineConstant[ N = {5, Min 2, Max 100, Step 1, Name "Parameters/0Number of slices"} dir = {0, Choices{0="X", 1="Y", 2="Z"}, Name "Parameters/1Direction"} surf = {0, Choices{0, 1}, Name "Parameters/2Keep only surfaces?"} ]; dx = (xmax - xmin); dy = (ymax - ymin); dz = (zmax - zmin); L = (dir == 0) ? dz : dx; H = (dir == 1) ? dz : dy; // Create the first cutting plane: s() = {news}; Rectangle(s(0)) = {xmin, ymin, zmin, L, H}; If(dir == 0) Rotate{ {0, 1, 0}, {xmin, ymin, zmin}, -Pi/2 } { Surface{s(0)}; } ElseIf(dir == 1) Rotate{ {1, 0, 0}, {xmin, ymin, zmin}, Pi/2 } { Surface{s(0)}; } EndIf tx = (dir == 0) ? dx / N : 0; ty = (dir == 1) ? dy / N : 0; tz = (dir == 2) ? dz / N : 0; Translate{tx, ty, tz} { Surface{s(0)}; } // Create the other cutting planes: For i In {1:N-2} s() += Translate{i * tx, i * ty, i * tz} { Duplicata{ Surface{s(0)}; } }; EndFor // Fragment (i.e. intersect) the volume with all the cutting planes: BooleanFragments{ Volume{v()}; Delete; }{ Surface{s()}; Delete; } // Now remove all the surfaces (and their bounding entities) that are not on the // boundary of a volume, i.e. the parts of the cutting planes that "stick out" // of the volume: Recursive Delete { Surface{:}; } If(surf) // If we want to only keep the surfaces, retrieve the surfaces in bounding // boxes around the cutting planes... eps = 1e-4; s() = {}; For i In {1:N-1} xx = (dir == 0) ? xmin : xmax; yy = (dir == 1) ? ymin : ymax; zz = (dir == 2) ? zmin : zmax; s() += Surface In BoundingBox {xmin - eps + i * tx, ymin - eps + i * ty, zmin - eps + i * tz, xx + eps + i * tx, yy + eps + i * ty, zz + eps + i * tz}; EndFor // ...and remove all the other entities: dels = Surface{:}; dels -= s(); Delete { Volume{:}; Surface{dels()}; Curve{:}; Point{:}; } EndIf // Finally, let's specify a global mesh size: Mesh.MeshSizeMin = 3; Mesh.MeshSizeMax = 3; // To partition the mesh instead of the geometry, see `t21.geo'.
Next: x1
: Geometry and mesh data, Previous: t20
: STEP import and manipulation, geometry partitioning, Up: Tutorial [Contents][Index]
t21
: Mesh partitioningSee t21.geo. Also available in C++ (t21.cpp) and Python (t21.py).
// ----------------------------------------------------------------------------- // // Gmsh GEO tutorial 21 // // Mesh partitioning // // ----------------------------------------------------------------------------- // Gmsh can partition meshes using different algorithms, e.g. the graph // partitioner Metis or the `SimplePartition' plugin. For all the partitining // algorithms, the relationship between mesh elements and mesh partitions is // encoded through the creation of new (discrete) elementary entities, called // "partition entities". // // Partition entities behave exactly like other discrete elementary entities; // the only difference is that they keep track of both a mesh partition index // and their parent elementary entity. // // The major advantage of this approach is that it allows to maintain a full // boundary representation of the partition entities, which Gmsh creates // automatically if `Mesh.PartitionCreateTopology' is set. // Let us start by creating a simple geometry with two adjacent squares sharing // an edge: SetFactory("OpenCASCADE"); Rectangle(1) = {0, 0, 0, 1, 1}; Rectangle(2) = {1, 0, 0, 1, 1}; BooleanFragments{ Surface{1}; Delete; }{ Surface{2}; Delete; } MeshSize {:} = 0.05; // We create one physical group for each square, and we mesh the resulting // geometry: Physical Surface("Left", 100) = 1; Physical Surface("Right", 200) = 2; Mesh 2; // We now define several constants to fine-tune how the mesh will be partitioned DefineConstant[ partitioner = {0, Choices{0="Metis", 1="SimplePartition"}, Name "Parameters/0Mesh partitioner"} N = {3, Min 1, Max 256, Step 1, Name "Parameters/1Number of partitions"} topology = {1, Choices{0, 1}, Name "Parameters/2Create partition topology (BRep)?"} ghosts = {0, Choices{0, 1}, Name "Parameters/3Create ghost cells?"} physicals = {0, Choices{0, 1}, Name "Parameters/3Create new physical groups?"} write = {1, Choices {0, 1}, Name "Parameters/3Write file to disk?"} split = {0, Choices {0, 1}, Name "Parameters/4Write one file per partition?"} ]; // Should we create the boundary representation of the partition entities? Mesh.PartitionCreateTopology = topology; // Should we create ghost cells? Mesh.PartitionCreateGhostCells = ghosts; // Should we automatically create new physical groups on the partition entities? Mesh.PartitionCreatePhysicals = physicals; // Should we keep backward compatibility with pre-Gmsh 4, e.g. to save the mesh // in MSH2 format? Mesh.PartitionOldStyleMsh2 = 0; // Should we save one mesh file per partition? Mesh.PartitionSplitMeshFiles = split; If (partitioner == 0) // Use Metis to create N partitions PartitionMesh N; // Several options can be set to control Metis: `Mesh.MetisAlgorithm' (1: // Recursive, 2: K-way), `Mesh.MetisObjective' (1: min. edge-cut, 2: // min. communication volume), `Mesh.PartitionTriWeight' (weight of // triangles), `Mesh.PartitionQuadWeight' (weight of quads), ... Else // Use the `SimplePartition' plugin to create chessboard-like partitions Plugin(SimplePartition).NumSlicesX = N; Plugin(SimplePartition).NumSlicesY = 1; Plugin(SimplePartition).NumSlicesZ = 1; Plugin(SimplePartition).Run; EndIf // Save mesh file (or files, if `Mesh.PartitionSplitMeshFiles' is set): If(write) Save "t21.msh"; EndIf
Next: x2
: Mesh import, discrete entities, hybrid models, terrain meshing, Previous: t21
: Mesh partitioning, Up: Tutorial [Contents][Index]
x1
: Geometry and mesh dataSee x1.py. Also available in C++ (x1.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 1 # # Geometry and mesh data # # ----------------------------------------------------------------------------- # The Python API allows to do much more than what can be done in .geo files. These # additional features are introduced gradually in the extended tutorials, # starting with `x1.py'. # In this first extended tutorial, we start by using the API to access basic # geometrical and mesh data. import gmsh import sys if len(sys.argv) < 2: print("Usage: " + sys.argv[0] + " file") exit gmsh.initialize() # You can run this tutorial on any file that Gmsh can read, e.g. a mesh file in # the MSH format: `python t1.py file.msh' gmsh.open(sys.argv[1]) # Print the model name and dimension: print('Model ' + gmsh.model.getCurrent() + ' (' + str(gmsh.model.getDimension()) + 'D)') # Geometrical data is made of elementary model `entities', called `points' # (entities of dimension 0), `curves' (entities of dimension 1), `surfaces' # (entities of dimension 2) and `volumes' (entities of dimension 3). As we have # seen in the other Python tutorials, elementary model entities are identified # by their dimension and by a `tag': a strictly positive identification # number. Model entities can be either CAD entities (from the built-in `geo' # kernel or from the OpenCASCADE `occ' kernel) or `discrete' entities (defined # by a mesh). `Physical groups' are collections of model entities and are also # identified by their dimension and by a tag. # Get all the elementary entities in the model, as a vector of (dimension, tag) # pairs: entities = gmsh.model.getEntities() for e in entities: # Dimension and tag of the entity: dim = e[0] tag = e[1] # Mesh data is made of `elements' (points, lines, triangles, ...), defined # by an ordered list of their `nodes'. Elements and nodes are identified by # `tags' as well (strictly positive identification numbers), and are stored # ("classified") in the model entity they discretize. Tags for elements and # nodes are globally unique (and not only per dimension, like entities). # A model entity of dimension 0 (a geometrical point) will contain a mesh # element of type point, as well as a mesh node. A model curve will contain # line elements as well as its interior nodes, while its boundary nodes will # be stored in the bounding model points. A model surface will contain # triangular and/or quadrangular elements and all the nodes not classified # on its boundary or on its embedded entities. A model volume will contain # tetrahedra, hexahedra, etc. and all the nodes not classified on its # boundary or on its embedded entities. # Get the mesh nodes for the entity (dim, tag): nodeTags, nodeCoords, nodeParams = gmsh.model.mesh.getNodes(dim, tag) # Get the mesh elements for the entity (dim, tag): elemTypes, elemTags, elemNodeTags = gmsh.model.mesh.getElements(dim, tag) # Elements can also be obtained by type, by using `getElementTypes()' # followed by `getElementsByType()'. # Let's print a summary of the information available on the entity and its # mesh. # * Type and name of the entity: type = gmsh.model.getType(e[0], e[1]) name = gmsh.model.getEntityName(e[0], e[1]) if len(name): name += ' ' print("Entity " + name + str(e) + " of type " + type) # * Number of mesh nodes and elements: numElem = sum(len(i) for i in elemTags) print(" - Mesh has " + str(len(nodeTags)) + " nodes and " + str(numElem) + " elements") # * Upward and downward adjacencies: up, down = gmsh.model.getAdjacencies(e[0], e[1]) if len(up): print(" - Upward adjacencies: " + str(up)) if len(down): print(" - Downward adjacencies: " + str(down)) # * Does the entity belong to physical groups? physicalTags = gmsh.model.getPhysicalGroupsForEntity(dim, tag) if len(physicalTags): s = '' for p in physicalTags: n = gmsh.model.getPhysicalName(dim, p) if n: n += ' ' s += n + '(' + str(dim) + ', ' + str(p) + ') ' print(" - Physical groups: " + s) # * Is the entity a partition entity? If so, what is its parent entity? partitions = gmsh.model.getPartitions(e[0], e[1]) if len(partitions): print(" - Partition tags: " + str(partitions) + " - parent entity " + str(gmsh.model.getParent(e[0], e[1]))) # * List all types of elements making up the mesh of the entity: for t in elemTypes: name, dim, order, numv, parv, _ = gmsh.model.mesh.getElementProperties( t) print(" - Element type: " + name + ", order " + str(order) + " (" + str(numv) + " nodes in param coord: " + str(parv) + ")") # We can use this to clear all the model data: gmsh.clear() gmsh.finalize()
Next: x3
: Post-processing data import: list-based, Previous: x1
: Geometry and mesh data, Up: Tutorial [Contents][Index]
x2
: Mesh import, discrete entities, hybrid models, terrain meshingSee x2.py. Also available in C++ (x2.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 2 # # Mesh import, discrete entities, hybrid models, terrain meshing # # ----------------------------------------------------------------------------- import gmsh import sys import math # The API can be used to import a mesh without reading it from a file, by # creating nodes and elements on the fly and storing them in model # entities. These model entities can be existing CAD entities, or can be # discrete entities, entirely defined by the mesh. # # Discrete entities can be reparametrized (see `t13.py') so that they can be # remeshed later on; and they can also be combined with built-in CAD entities to # produce hybrid models. # # We combine all these features in this tutorial to perform terrain meshing, # where the terrain is described by a discrete surface (that we then # reparametrize) combined with a CAD representation of the underground. gmsh.initialize() gmsh.model.add("x2") # We will create the terrain surface mesh from N x N input data points: N = 100 # Helper function to return a node tag given two indices i and j: def tag(i, j): return (N + 1) * i + j + 1 # The x, y, z coordinates of all the nodes: coords = [] # The tags of the corresponding nodes: nodes = [] # The connectivities of the triangle elements (3 node tags per triangle) on the # terrain surface: tris = [] # The connectivities of the line elements on the 4 boundaries (2 node tags # for each line element): lin = [[], [], [], []] # The connectivities of the point elements on the 4 corners (1 node tag for each # point element): pnt = [tag(0, 0), tag(N, 0), tag(N, N), tag(0, N)] for i in range(N + 1): for j in range(N + 1): nodes.append(tag(i, j)) coords.extend([ float(i) / N, float(j) / N, 0.05 * math.sin(10 * float(i + j) / N) ]) if i > 0 and j > 0: tris.extend([tag(i - 1, j - 1), tag(i, j - 1), tag(i - 1, j)]) tris.extend([tag(i, j - 1), tag(i, j), tag(i - 1, j)]) if (i == 0 or i == N) and j > 0: lin[3 if i == 0 else 1].extend([tag(i, j - 1), tag(i, j)]) if (j == 0 or j == N) and i > 0: lin[0 if j == 0 else 2].extend([tag(i - 1, j), tag(i, j)]) # Create 4 discrete points for the 4 corners of the terrain surface: for i in range(4): gmsh.model.addDiscreteEntity(0, i + 1) gmsh.model.setCoordinates(1, 0, 0, coords[3 * tag(0, 0) - 1]) gmsh.model.setCoordinates(2, 1, 0, coords[3 * tag(N, 0) - 1]) gmsh.model.setCoordinates(3, 1, 1, coords[3 * tag(N, N) - 1]) gmsh.model.setCoordinates(4, 0, 1, coords[3 * tag(0, N) - 1]) # Create 4 discrete bounding curves, with their boundary points: for i in range(4): gmsh.model.addDiscreteEntity(1, i + 1, [i + 1, i + 2 if i < 3 else 1]) # Create one discrete surface, with its bounding curves: gmsh.model.addDiscreteEntity(2, 1, [1, 2, -3, -4]) # Add all the nodes on the surface (for simplicity... see below): gmsh.model.mesh.addNodes(2, 1, nodes, coords) # Add point elements on the 4 points, line elements on the 4 curves, and # triangle elements on the surface: for i in range(4): # Type 15 for point elements: gmsh.model.mesh.addElementsByType(i + 1, 15, [], [pnt[i]]) # Type 1 for 2-node line elements: gmsh.model.mesh.addElementsByType(i + 1, 1, [], lin[i]) # Type 2 for 3-node triangle elements: gmsh.model.mesh.addElementsByType(1, 2, [], tris) # Reclassify the nodes on the curves and the points (since we put them all on # the surface before with `addNodes' for simplicity) gmsh.model.mesh.reclassifyNodes() # Create a geometry for the discrete curves and surfaces, so that we can remesh # them later on: gmsh.model.mesh.createGeometry() # Note that for more complicated meshes, e.g. for on input unstructured STL # mesh, we could use `classifySurfaces()' to automatically create the discrete # entities and the topology; but we would then have to extract the boundaries # afterwards. # Create other build-in CAD entities to form one volume below the terrain # surface. Beware that only built-in CAD entities can be hybrid, i.e. have # discrete entities on their boundary: OpenCASCADE does not support this # feature. p1 = gmsh.model.geo.addPoint(0, 0, -0.5) p2 = gmsh.model.geo.addPoint(1, 0, -0.5) p3 = gmsh.model.geo.addPoint(1, 1, -0.5) p4 = gmsh.model.geo.addPoint(0, 1, -0.5) c1 = gmsh.model.geo.addLine(p1, p2) c2 = gmsh.model.geo.addLine(p2, p3) c3 = gmsh.model.geo.addLine(p3, p4) c4 = gmsh.model.geo.addLine(p4, p1) c10 = gmsh.model.geo.addLine(p1, 1) c11 = gmsh.model.geo.addLine(p2, 2) c12 = gmsh.model.geo.addLine(p3, 3) c13 = gmsh.model.geo.addLine(p4, 4) ll1 = gmsh.model.geo.addCurveLoop([c1, c2, c3, c4]) s1 = gmsh.model.geo.addPlaneSurface([ll1]) ll3 = gmsh.model.geo.addCurveLoop([c1, c11, -1, -c10]) s3 = gmsh.model.geo.addPlaneSurface([ll3]) ll4 = gmsh.model.geo.addCurveLoop([c2, c12, -2, -c11]) s4 = gmsh.model.geo.addPlaneSurface([ll4]) ll5 = gmsh.model.geo.addCurveLoop([c3, c13, 3, -c12]) s5 = gmsh.model.geo.addPlaneSurface([ll5]) ll6 = gmsh.model.geo.addCurveLoop([c4, c10, 4, -c13]) s6 = gmsh.model.geo.addPlaneSurface([ll6]) sl1 = gmsh.model.geo.addSurfaceLoop([s1, s3, s4, s5, s6, 1]) v1 = gmsh.model.geo.addVolume([sl1]) gmsh.model.geo.synchronize() # Set this to True to build a fully hex mesh: #transfinite = True transfinite = False transfiniteAuto = False if transfinite: NN = 30 for c in gmsh.model.getEntities(1): gmsh.model.mesh.setTransfiniteCurve(c[1], NN) for s in gmsh.model.getEntities(2): gmsh.model.mesh.setTransfiniteSurface(s[1]) gmsh.model.mesh.setRecombine(s[0], s[1]) gmsh.model.mesh.setSmoothing(s[0], s[1], 100) gmsh.model.mesh.setTransfiniteVolume(v1) elif transfiniteAuto: gmsh.option.setNumber('Mesh.MeshSizeMin', 0.5) gmsh.option.setNumber('Mesh.MeshSizeMax', 0.5) # setTransfiniteAutomatic() uses the sizing constraints to set the number # of points gmsh.model.mesh.setTransfiniteAutomatic() else: gmsh.option.setNumber('Mesh.MeshSizeMin', 0.05) gmsh.option.setNumber('Mesh.MeshSizeMax', 0.05) gmsh.model.mesh.generate(3) gmsh.write('x2.msh') # Launch the GUI to see the results: if '-nopopup' not in sys.argv: gmsh.fltk.run() gmsh.finalize()
Next: x4
: Post-processing data import: model-based, Previous: x2
: Mesh import, discrete entities, hybrid models, terrain meshing, Up: Tutorial [Contents][Index]
x3
: Post-processing data import: list-basedSee x3.py. Also available in C++ (x3.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 3 # # Post-processing data import: list-based # # ----------------------------------------------------------------------------- import gmsh import sys gmsh.initialize(sys.argv) # Gmsh supports two types of post-processing data: "list-based" and # "model-based". Both types of data are handled through the `view' interface. # List-based views are completely independent from any model and any mesh: they # are self-contained and simply contain lists of coordinates and values, element # by element, for 3 types of fields (scalar "S", vector "V" and tensor "T") and # several types of element shapes (point "P", line "L", triangle "T", quadrangle # "Q", tetrahedron "S", hexahedron "H", prism "I" and pyramid "Y"). (See `x4.py' # for a tutorial on model-based views.) # To create a list-based view one should first create a view: t1 = gmsh.view.add("A list-based view") # List-based data is then added by specifying the type as a 2 character string # that combines a field type and an element shape (e.g. "ST" for a scalar field # on triangles), the number of elements to be added, and the concatenated list # of coordinates (e.g. 3 "x" coordinates, 3 "y" coordinates, 3 "z" coordinates # for first order triangles) and values for each element (e.g. 3 values for # first order scalar triangles, repeated for each step if there are several time # steps). # Let's create two triangles... triangle1 = [0., 1., 1., # x coordinates of the 3 triangle nodes 0., 0., 1., # y coordinates of the 3 triangle nodes 0., 0., 0.] # z coordinates of the 3 triangle nodes triangle2 = [0., 1., 0., 0., 1., 1., 0., 0., 0.] # ... and append values for 10 time steps for step in range(0, 10): triangle1.extend([10., 11. - step, 12.]) # 3 node values for each step triangle2.extend([11., 12., 13. + step]) # List-based data is just added by concatenating the data for all the triangles: gmsh.view.addListData(t1, "ST", 2, triangle1 + triangle2) # Internally, post-processing views parsed by the .geo file parser create such # list-based data (see e.g. `t7.py', `t8.py' and `t9.py'), independently of any # mesh. # Vector or tensor fields can be imported in the same way, the only difference # beeing the type (starting with "V" for vector fields and "T" for tensor # fields) and the number of components. For example a vector field on a line # element can be added as follows: line = [ 0., 1., # x coordinate of the 2 line nodes 1.2, 1.2, # y coordinate of the 2 line nodes 0., 0. # z coordinate of the 2 line nodes ] for step in range(0, 10): # 3 vector components for each node (2 nodes here), for each step line.extend([10. + step, 0., 0., 10. + step, 0., 0.]) gmsh.view.addListData(t1, "VL", 1, line) # List-based data can also hold 2D (in window coordinates) and 3D (in model # coordinates) strings (see `t4.py'). Here we add a 2D string located on the # bottom-left of the window (with a 20 pixels offset), as well as a 3D string # located at model coordinates (0.5, 0.5. 0): gmsh.view.addListDataString(t1, [20., -20.], ["Created with Gmsh"]) gmsh.view.addListDataString(t1, [0.5, 1.5, 0.], ["A multi-step list-based view"], ["Align", "Center", "Font", "Helvetica"]) # The various attributes of the view can be queried and changed using the option # interface. Beware that the option interface uses view indices instead of view # tags; so to change the current time step and the intervals type, and to # retrieve the total number of steps, one would do: v1 = "View[" + str(gmsh.view.getIndex(t1)) + "]" gmsh.option.setNumber(v1 + ".TimeStep", 5) gmsh.option.setNumber(v1 + ".IntervalsType", 3) ns = gmsh.option.getNumber(v1 + ".NbTimeStep") print(v1 + " with tag " + str(t1) + " has " + str(ns) + " time steps") # Views can be queried and modified in various ways using plugins (see `t9.py'), # or probed directly using `gmsh.view.probe()' - here at point (0.9, 0.1, 0): print("Value at (0.9, 0.1, 0)", gmsh.view.probe(t1, 0.9, 0.1, 0)) # Views can be saved to disk using `gmsh.view.write()': gmsh.view.write(t1, "x3.pos") # High-order datasets can be provided by setting the interpolation matrices # explicitly. Let's create a second view with second order interpolation on # a 4-node quadrangle. # Add a new view: t2 = gmsh.view.add("Second order quad") # Set the node coordinates: quad = [0., 1., 1., 0., # x coordinates of the 4 quadrangle nodes -1.2, -1.2, -0.2, -0.2, # y coordinates of the 4 quadrangle nodes 0., 0., 0., 0.] # z coordinates of the 4 quadrangle nodes # Add nine values that will be interpolated by second order basis functions quad.extend([1., 1., 1., 1., 3., 3., 3., 3., -3.]) # Set the two interpolation matrices c[i][j] and e[i][j] defining the d = 9 # basis functions: f[i](u, v, w) = sum_(j = 0, ..., d - 1) c[i][j] u^e[j][0] # v^e[j][1] w^e[j][2], i = 0, ..., d-1, with u, v, w the coordinates in the # reference element: gmsh.view.setInterpolationMatrices(t2, "Quadrangle", 9, [0, 0, 0.25, 0, 0, -0.25, -0.25, 0, 0.25, 0, 0, 0.25, 0, 0, -0.25, 0.25, 0, -0.25, 0, 0, 0.25, 0, 0, 0.25, 0.25, 0, 0.25, 0, 0, 0.25, 0, 0, 0.25, -0.25, 0, -0.25, 0, 0, -0.5, 0.5, 0, 0.5, 0, -0.5, 0, 0, 0.5, -0.5, 0, 0.5, 0, -0.5, 0, 0, 0, 0, -0.5, 0.5, 0, -0.5, 0, 0.5, 0, 0, 0.5, -0.5, 0, -0.5, 0, 0.5, 0, 0, 1, -1, 1, -1, 0, 0, 0, 0, 0], [0, 0, 0, 2, 0, 0, 2, 2, 0, 0, 2, 0, 1, 0, 0, 2, 1, 0, 1, 2, 0, 0, 1, 0, 1, 1, 0]) # Note that two additional interpolation matrices could also be provided to # interpolate the geometry, i.e. to interpolate curved elements. # Add the data to the view: gmsh.view.addListData(t2, "SQ", 1, quad) # In order to visualize the high-order field, one must activate adaptive # visualization, set a visualization error threshold and a maximum subdivision # level (Gmsh does automatic mesh refinement to visualize the high-order field # with the requested accuracy): v2 = "View[" + str(gmsh.view.getIndex(t2)) + "]" gmsh.option.setNumber(v2 + ".AdaptVisualizationGrid", 1) gmsh.option.setNumber(v2 + ".TargetError", 1e-2) gmsh.option.setNumber(v2 + ".MaxRecursionLevel", 5) # Launch the GUI to see the results: if '-nopopup' not in sys.argv: gmsh.fltk.run() gmsh.finalize()
Previous: x3
: Post-processing data import: list-based, Up: Tutorial [Contents][Index]
x4
: Post-processing data import: model-basedSee x4.py. Also available in C++ (x4.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 4 # # Post-processing data import: model-based # # ----------------------------------------------------------------------------- import gmsh import sys gmsh.initialize(sys.argv) # Contrary to list-based view (see `x3.py'), model-based views are based on one # or more meshes. Compared to list-based views, they are thus linked to one # model (per step). Post-processing data stored in MSH files create such # model-based views. # Let's create a first model-based view using a simple mesh contructed by # hand. We create a model with a discrete surface gmsh.model.add("simple model") surf = gmsh.model.addDiscreteEntity(2) # We add 4 nodes and 2 3-node triangles (element type "2") gmsh.model.mesh.addNodes(2, surf, [1, 2, 3, 4], [0., 0., 0., 1., 0., 0., 1., 1., 0., 0., 1., 0.]) gmsh.model.mesh.addElementsByType(surf, 2, [1, 2], [1, 2, 3, 1, 3, 4]) # We can now create a new model-based view, to which we add 10 steps of # node-based data: t1 = gmsh.view.add("A model-based view") for step in range(0, 10): gmsh.view.addHomogeneousModelData( t1, step, "simple model", "NodeData", [1, 2, 3, 4], # tags of nodes [10., 10., 12. + step, 13. + step]) # data, per node # Besided node-based data, which result in continuous fields, one can also add # general discontinous fields defined at the nodes of each element, using # "ElementNodeData": t2 = gmsh.view.add("A discontinuous model-based view") for step in range(0, 10): gmsh.view.addHomogeneousModelData( t2, step, "simple model", "ElementNodeData", [1, 2], # tags of elements [10., 10., 12. + step, 14., 15., 13. + step]) # data per element nodes # Constant per element datasets can also be created using "ElementData". Note # that a more general function `addModelData' to add data for hybrid meshes # (when data is not homogeneous, i.e. when the number of nodes changes between # elements) is also available. # Each step of a model-based view can be defined on a different model, i.e. on a # different mesh. Let's define a second model and mesh it gmsh.model.add("another model") gmsh.model.occ.addBox(0, 0, 0, 1, 1, 1) gmsh.model.occ.synchronize() gmsh.model.mesh.generate(3) # We can add other steps to view "t" based on this new mesh: nodes, coord, _ = gmsh.model.mesh.getNodes() for step in range(11, 20): gmsh.view.addHomogeneousModelData( t1, step, "another model", "NodeData", nodes, [step * coord[i] for i in range(0, len(coord), 3)]) # This feature allows to create seamless animations for time-dependent datasets # on deforming or remeshed models. # High-order node-based datasets are supported without needing to supply the # interpolation matrices (iso-parametric Lagrange elements). Arbitrary # high-order datasets can be specified as "ElementNodeData", with the # interpolation matrices specified in the same as as for list-based views (see # `x3.py'). # Model-based views can be saved to disk using `gmsh.view.write()'; note that # saving a view based on multiple meshes (like the view `t1') will automatically # create several files. If the `PostProcessing.SaveMesh' option is not set, # `gmsh.view.write()' will only save the view data, without the mesh (which # could be saved independently with `gmsh.write()'). gmsh.view.write(t1, "x4_t1.msh") gmsh.view.write(t2, "x4_t2.msh") # Launch the GUI to see the results: if '-nopopup' not in sys.argv: gmsh.fltk.run() gmsh.finalize()
Next: Compiling the source code, Previous: Tutorial, Up: Gmsh [Contents][Index]
This appendix lists all the available options. Gmsh’s default behavior
is to save some of these options in a per-user “session resource” file
(cf. “Saved in: General.SessionFileName
” in the lists below)
every time Gmsh is shut down. This permits for example to automatically
remember the size and location of the windows or which fonts to use. A
second set of options can be saved (automatically or manually with the
‘File->Save Options As Default’ menu) in a per-user “option” file
(cf. “Saved in: General.OptionsFileName
” in the lists below),
automatically loaded by Gmsh every time it starts up. Finally, other
options are only saved to disk manually, either by explicitly saving an
option file with ‘File->Export’, or when saving per-model options with
‘File->Save Model Options’ (cf. “Saved in: -
” in the lists
below).
To reset all options to their default values, use ‘Help->Restore All
Options to Default Settings’ or the ‘Restore all options to default
settings’ button in ‘Tools->Options->General->Advanced’, or erase the
General.SessionFileName
and General.OptionsFileName
files
by hand.
All the options can be manipulated through the Gmsh API through the
gmsh/option
namespace (see Gmsh API).
Next: Geometry options list, Previous: Options, Up: Options [Contents][Index]
General.AxesFormatX
¶Number format for X-axis (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
General.AxesFormatY
¶Number format for Y-axis (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
General.AxesFormatZ
¶Number format for Z-axis (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
General.AxesLabelX
¶X-axis label
Default value: ""
Saved in: General.OptionsFileName
General.AxesLabelY
¶Y-axis label
Default value: ""
Saved in: General.OptionsFileName
General.AxesLabelZ
¶Z-axis label
Default value: ""
Saved in: General.OptionsFileName
General.BackgroundImageFileName
¶Background image file in JPEG, PNG or PDF format
Default value: ""
Saved in: General.OptionsFileName
General.BuildInfo
¶Gmsh build information (read-only)
Default value: "Version: 4.8.2-git-f4a047dba; License: GNU General Public License; Build OS: MacOSX-sdk; Build date: 20210326; Build host: Mac-mini.local; Build options: 64Bit ALGLIB ANN Bamg Blossom DIntegration Dlopen DomHex Eigen Fltk Gmm Hxt Jpeg[fltk] Kbipack MathEx Mesh Metis Mpeg Netgen ONELAB ONELABMetamodel OpenGL OptHom Parser Plugins Png[fltk] Post QuadMeshingTools QuadTri Solver TetGen/BR TouchBar Voro++ Zlib; FLTK version: 1.4.0; Packaged by: geuzaine; Web site: https://gmsh.info; Issue tracker: https://gitlab.onelab.info/gmsh/gmsh/issues"
Saved in: -
General.BuildOptions
¶Gmsh build options (read-only)
Default value: "64Bit ALGLIB ANN Bamg Blossom DIntegration Dlopen DomHex Eigen Fltk Gmm Hxt Jpeg[fltk] Kbipack MathEx Mesh Metis Mpeg Netgen ONELAB ONELABMetamodel OpenGL OptHom Parser Plugins Png[fltk] Post QuadMeshingTools QuadTri Solver TetGen/BR TouchBar Voro++ Zlib"
Saved in: -
General.DefaultFileName
¶Default project file name
Default value: "untitled.geo"
Saved in: General.OptionsFileName
General.Display
¶X server to use (only for Unix versions)
Default value: ""
Saved in: -
General.ErrorFileName
¶File into which the log is saved if a fatal error occurs
Default value: ".gmsh-errors"
Saved in: General.OptionsFileName
General.ExecutableFileName
¶File name of the Gmsh executable (read-only)
Default value: ""
Saved in: General.SessionFileName
General.FileName
¶Current project file name (read-only)
Default value: ""
Saved in: -
General.FltkTheme
¶FLTK user interface theme (try e.g. plastic or gtk+)
Default value: ""
Saved in: General.SessionFileName
General.GraphicsFont
¶Font used in the graphic window
Default value: "Helvetica"
Saved in: General.OptionsFileName
General.GraphicsFontEngine
¶Set graphics font engine (Native, StringTexture, Cairo)
Default value: "Native"
Saved in: General.OptionsFileName
General.GraphicsFontTitle
¶Font used in the graphic window for titles
Default value: "Helvetica"
Saved in: General.OptionsFileName
General.OptionsFileName
¶Option file created with ‘Tools->Options->Save’; automatically read on startup
Default value: ".gmsh-options"
Saved in: General.SessionFileName
General.RecentFile0
¶Most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile1
¶2nd most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile2
¶3rd most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile3
¶4th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile4
¶5th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile5
¶6th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile6
¶7th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile7
¶8th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile8
¶9th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.RecentFile9
¶10th most recent opened file
Default value: "untitled.geo"
Saved in: General.SessionFileName
General.SessionFileName
¶Option file into which session specific information is saved; automatically read on startup
Default value: ".gmshrc"
Saved in: -
General.ScriptingLanguages
¶Language(s) in which scripting commands generated by the GUI are written
Default value: "geo"
Saved in: General.OptionsFileName
General.TextEditor
¶System command to launch a text editor
Default value: "open -t '%s'"
Saved in: General.OptionsFileName
General.TmpFileName
¶Temporary file used by the geometry module
Default value: ".gmsh-tmp"
Saved in: General.SessionFileName
General.Version
¶Gmsh version (read-only)
Default value: "4.8.2-git-f4a047dba"
Saved in: -
General.WatchFilePattern
¶Pattern of files to merge as they become available
Default value: ""
Saved in: -
General.AbortOnError
¶Abort on error? (0: no, 1: abort meshing, 2: throw an exception unless in interactive mode, 3: throw an exception always, 4: exit)
Default value: 0
Saved in: General.OptionsFileName
General.AlphaBlending
¶Enable alpha blending (transparency) in post-processing views
Default value: 1
Saved in: General.OptionsFileName
General.Antialiasing
¶Use multisample antialiasing (will slow down rendering)
Default value: 0
Saved in: General.OptionsFileName
General.ArrowHeadRadius
¶Relative radius of arrow head
Default value: 0.12
Saved in: General.OptionsFileName
General.ArrowStemLength
¶Relative length of arrow stem
Default value: 0.56
Saved in: General.OptionsFileName
General.ArrowStemRadius
¶Relative radius of arrow stem
Default value: 0.02
Saved in: General.OptionsFileName
General.Axes
¶Axes (0: none, 1: simple axes, 2: box, 3: full grid, 4: open grid, 5: ruler)
Default value: 0
Saved in: General.OptionsFileName
General.AxesMikado
¶Mikado axes style
Default value: 0
Saved in: General.OptionsFileName
General.AxesAutoPosition
¶Position the axes automatically
Default value: 1
Saved in: General.OptionsFileName
General.AxesForceValue
¶Force values on axes (otherwise use natural coordinates)
Default value: 0
Saved in: General.OptionsFileName
General.AxesMaxX
¶Maximum X-axis coordinate
Default value: 1
Saved in: General.OptionsFileName
General.AxesMaxY
¶Maximum Y-axis coordinate
Default value: 1
Saved in: General.OptionsFileName
General.AxesMaxZ
¶Maximum Z-axis coordinate
Default value: 1
Saved in: General.OptionsFileName
General.AxesMinX
¶Minimum X-axis coordinate
Default value: 0
Saved in: General.OptionsFileName
General.AxesMinY
¶Minimum Y-axis coordinate
Default value: 0
Saved in: General.OptionsFileName
General.AxesMinZ
¶Minimum Z-axis coordinate
Default value: 0
Saved in: General.OptionsFileName
General.AxesTicsX
¶Number of tics on the X-axis
Default value: 5
Saved in: General.OptionsFileName
General.AxesTicsY
¶Number of tics on the Y-axis
Default value: 5
Saved in: General.OptionsFileName
General.AxesTicsZ
¶Number of tics on the Z-axis
Default value: 5
Saved in: General.OptionsFileName
General.AxesValueMaxX
¶Maximum X-axis forced value
Default value: 1
Saved in: General.OptionsFileName
General.AxesValueMaxY
¶Maximum Y-axis forced value
Default value: 1
Saved in: General.OptionsFileName
General.AxesValueMaxZ
¶Maximum Z-axis forced value
Default value: 1
Saved in: General.OptionsFileName
General.AxesValueMinX
¶Minimum X-axis forced value
Default value: 0
Saved in: General.OptionsFileName
General.AxesValueMinY
¶Minimum Y-axis forced value
Default value: 0
Saved in: General.OptionsFileName
General.AxesValueMinZ
¶Minimum Z-axis forced value
Default value: 0
Saved in: General.OptionsFileName
General.BackgroundGradient
¶Draw background gradient (0: none, 1: vertical, 2: horizontal, 3: radial)
Default value: 1
Saved in: General.OptionsFileName
General.BackgroundImage3D
¶Create background image in the 3D model (units = model units) or as 2D background (units = pixels)
Default value: 0
Saved in: General.OptionsFileName
General.BackgroundImagePage
¶Page to render in the background image (for multi-page PDFs)
Default value: 0
Saved in: General.OptionsFileName
General.BackgroundImagePositionX
¶X position of background image (for 2D background: < 0: measure from right window edge; >= 1e5: centered)
Default value: 0
Saved in: General.OptionsFileName
General.BackgroundImagePositionY
¶Y position of background image (for 2D background: < 0: measure from bottom window edge; >= 1e5: centered)
Default value: 0
Saved in: General.OptionsFileName
General.BackgroundImageWidth
¶Width of background image (0: actual width if height = 0, natural scaling if not; -1: graphic window width)
Default value: -1
Saved in: General.OptionsFileName
General.BackgroundImageHeight
¶Height of background image (0: actual height if width = 0, natural scaling if not; -1: graphic window height)
Default value: -1
Saved in: General.OptionsFileName
General.BoundingBoxSize
¶Overall bounding box size (read-only)
Default value: 1
Saved in: General.OptionsFileName
General.Camera
¶Enable camera view mode
Default value: 0
Saved in: General.OptionsFileName
General.CameraAperture
¶Camera aperture in degrees
Default value: 40
Saved in: General.OptionsFileName
General.CameraEyeSeparationRatio
¶Eye separation ratio in % for stereo rendering
Default value: 1.5
Saved in: General.OptionsFileName
General.CameraFocalLengthRatio
¶Camera Focal length ratio
Default value: 1
Saved in: General.OptionsFileName
General.Clip0A
¶First coefficient in equation for clipping plane 0 (‘A’ in ‘AX+BY+CZ+D=0’)
Default value: 1
Saved in: -
General.Clip0B
¶Second coefficient in equation for clipping plane 0 (‘B’ in ‘AX+BY+CZ+D=0’)
Default value: 0
Saved in: -
General.Clip0C
¶Third coefficient in equation for clipping plane 0 (‘C’ in ‘AX+BY+CZ+D=0’)
Default value: 0
Saved in: -
General.Clip0D
¶Fourth coefficient in equation for clipping plane 0 (‘D’ in ‘AX+BY+CZ+D=0’)
Default value: 0
Saved in: -
General.Clip1A
¶First coefficient in equation for clipping plane 1
Default value: 0
Saved in: -
General.Clip1B
¶Second coefficient in equation for clipping plane 1
Default value: 1
Saved in: -
General.Clip1C
¶Third coefficient in equation for clipping plane 1
Default value: 0
Saved in: -
General.Clip1D
¶Fourth coefficient in equation for clipping plane 1
Default value: 0
Saved in: -
General.Clip2A
¶First coefficient in equation for clipping plane 2
Default value: 0
Saved in: -
General.Clip2B
¶Second coefficient in equation for clipping plane 2
Default value: 0
Saved in: -
General.Clip2C
¶Third coefficient in equation for clipping plane 2
Default value: 1
Saved in: -
General.Clip2D
¶Fourth coefficient in equation for clipping plane 2
Default value: 0
Saved in: -
General.Clip3A
¶First coefficient in equation for clipping plane 3
Default value: -1
Saved in: -
General.Clip3B
¶Second coefficient in equation for clipping plane 3
Default value: 0
Saved in: -
General.Clip3C
¶Third coefficient in equation for clipping plane 3
Default value: 0
Saved in: -
General.Clip3D
¶Fourth coefficient in equation for clipping plane 3
Default value: 1
Saved in: -
General.Clip4A
¶First coefficient in equation for clipping plane 4
Default value: 0
Saved in: -
General.Clip4B
¶Second coefficient in equation for clipping plane 4
Default value: -1
Saved in: -
General.Clip4C
¶Third coefficient in equation for clipping plane 4
Default value: 0
Saved in: -
General.Clip4D
¶Fourth coefficient in equation for clipping plane 4
Default value: 1
Saved in: -
General.Clip5A
¶First coefficient in equation for clipping plane 5
Default value: 0
Saved in: -
General.Clip5B
¶Second coefficient in equation for clipping plane 5
Default value: 0
Saved in: -
General.Clip5C
¶Third coefficient in equation for clipping plane 5
Default value: -1
Saved in: -
General.Clip5D
¶Fourth coefficient in equation for clipping plane 5
Default value: 1
Saved in: -
General.ClipFactor
¶Near and far clipping plane distance factor (decrease value for better z-buffer resolution)
Default value: 5
Saved in: -
General.ClipOnlyDrawIntersectingVolume
¶Only draw layer of elements that intersect the clipping plane
Default value: 0
Saved in: General.OptionsFileName
General.ClipOnlyVolume
¶Only clip volume elements
Default value: 0
Saved in: General.OptionsFileName
General.ClipPositionX
¶Horizontal position (in pixels) of the upper left corner of the clipping planes window
Default value: 650
Saved in: General.SessionFileName
General.ClipPositionY
¶Vertical position (in pixels) of the upper left corner of the clipping planes window
Default value: 150
Saved in: General.SessionFileName
General.ClipWholeElements
¶Clip whole elements
Default value: 0
Saved in: General.OptionsFileName
General.ColorScheme
¶Default color scheme for graphics (0: light, 1: default, 2: grayscale, 3: dark)
Default value: 1
Saved in: General.SessionFileName
General.ConfirmOverwrite
¶Ask confirmation before overwriting files?
Default value: 1
Saved in: General.OptionsFileName
General.ContextPositionX
¶Horizontal position (in pixels) of the upper left corner of the contextual windows
Default value: 650
Saved in: General.SessionFileName
General.ContextPositionY
¶Vertical position (in pixels) of the upper left corner of the contextual windows
Default value: 150
Saved in: General.SessionFileName
General.DetachedMenu
¶Should the menu window be detached from the graphic window?
Default value: 0
Saved in: General.SessionFileName
General.DisplayBorderFactor
¶Border factor for model display (0: model fits window size exactly)
Default value: 0.2
Saved in: General.OptionsFileName
General.DoubleBuffer
¶Use a double buffered graphic window (on Unix, should be set to 0 when working on a remote host without GLX)
Default value: 1
Saved in: General.OptionsFileName
General.DrawBoundingBoxes
¶Draw bounding boxes
Default value: 0
Saved in: General.OptionsFileName
General.ExpertMode
¶Enable expert mode (to disable all the messages meant for inexperienced users)
Default value: 0
Saved in: General.OptionsFileName
General.ExtraPositionX
¶Horizontal position (in pixels) of the upper left corner of the generic extra window
Default value: 650
Saved in: General.SessionFileName
General.ExtraPositionY
¶Vertical position (in pixels) of the upper left corner of the generic extra window
Default value: 350
Saved in: General.SessionFileName
General.ExtraHeight
¶Height (in pixels) of the generic extra window
Default value: 100
Saved in: General.SessionFileName
General.ExtraWidth
¶Width (in pixels) of the generic extra window
Default value: 100
Saved in: General.SessionFileName
General.FastRedraw
¶Draw simplified model while rotating, panning and zooming
Default value: 0
Saved in: General.OptionsFileName
General.FieldPositionX
¶Horizontal position (in pixels) of the upper left corner of the field window
Default value: 650
Saved in: General.SessionFileName
General.FieldPositionY
¶Vertical position (in pixels) of the upper left corner of the field window
Default value: 550
Saved in: General.SessionFileName
General.FieldHeight
¶Height (in pixels) of the field window
Default value: 320
Saved in: General.SessionFileName
General.FieldWidth
¶Width (in pixels) of the field window
Default value: 420
Saved in: General.SessionFileName
General.FileChooserPositionX
¶Horizontal position (in pixels) of the upper left corner of the file chooser windows
Default value: 200
Saved in: General.SessionFileName
General.FileChooserPositionY
¶Vertical position (in pixels) of the upper left corner of the file chooser windows
Default value: 200
Saved in: General.SessionFileName
General.FltkColorScheme
¶FLTK user interface color theme (0: standard, 1:dark)
Default value: 0
Saved in: General.SessionFileName
General.FltkRefreshRate
¶FLTK user interface maximum refresh rate, per second (0: no limit)
Default value: 5
Saved in: General.OptionsFileName
General.FontSize
¶Size of the font in the user interface, in pixels (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
General.GraphicsFontSize
¶Size of the font in the graphic window, in pixels
Default value: 15
Saved in: General.OptionsFileName
General.GraphicsFontSizeTitle
¶Size of the font in the graphic window for titles, in pixels
Default value: 18
Saved in: General.OptionsFileName
General.GraphicsHeight
¶Height (in pixels) of the graphic window
Default value: 600
Saved in: General.SessionFileName
General.GraphicsPositionX
¶Horizontal position (in pixels) of the upper left corner of the graphic window
Default value: 50
Saved in: General.SessionFileName
General.GraphicsPositionY
¶Vertical position (in pixels) of the upper left corner of the graphic window
Default value: 50
Saved in: General.SessionFileName
General.GraphicsWidth
¶Width (in pixels) of the graphic window
Default value: 800
Saved in: General.SessionFileName
General.HighOrderToolsPositionX
¶Horizontal position (in pixels) of the upper left corner of the high-order tools window
Default value: 650
Saved in: General.SessionFileName
General.HighOrderToolsPositionY
¶Vertical position (in pixels) of the upper left corner of the high-order tools window
Default value: 150
Saved in: General.SessionFileName
General.HighResolutionGraphics
¶Use high-resolution OpenGL graphics (e.g. for Macs with retina displays)
Default value: 1
Saved in: General.OptionsFileName
General.InitialModule
¶Module launched on startup (0: automatic, 1: geometry, 2: mesh, 3: solver, 4: post-processing)
Default value: 0
Saved in: General.OptionsFileName
General.InputScrolling
¶Enable numerical input scrolling in user interface (moving the mouse to change numbers)
Default value: 1
Saved in: General.OptionsFileName
General.Light0
¶Enable light source 0
Default value: 1
Saved in: General.OptionsFileName
General.Light0X
¶X position of light source 0
Default value: 0.65
Saved in: General.OptionsFileName
General.Light0Y
¶Y position of light source 0
Default value: 0.65
Saved in: General.OptionsFileName
General.Light0Z
¶Z position of light source 0
Default value: 1
Saved in: General.OptionsFileName
General.Light0W
¶Divisor of the X, Y and Z coordinates of light source 0 (W=0 means infinitely far source)
Default value: 0
Saved in: General.OptionsFileName
General.Light1
¶Enable light source 1
Default value: 0
Saved in: General.OptionsFileName
General.Light1X
¶X position of light source 1
Default value: 0.5
Saved in: General.OptionsFileName
General.Light1Y
¶Y position of light source 1
Default value: 0.3
Saved in: General.OptionsFileName
General.Light1Z
¶Z position of light source 1
Default value: 1
Saved in: General.OptionsFileName
General.Light1W
¶Divisor of the X, Y and Z coordinates of light source 1 (W=0 means infinitely far source)
Default value: 0
Saved in: General.OptionsFileName
General.Light2
¶Enable light source 2
Default value: 0
Saved in: General.OptionsFileName
General.Light2X
¶X position of light source 2
Default value: 0.5
Saved in: General.OptionsFileName
General.Light2Y
¶Y position of light source 2
Default value: 0.3
Saved in: General.OptionsFileName
General.Light2Z
¶Z position of light source 2
Default value: 1
Saved in: General.OptionsFileName
General.Light2W
¶Divisor of the X, Y and Z coordinates of light source 2 (W=0 means infinitely far source)
Default value: 0
Saved in: General.OptionsFileName
General.Light3
¶Enable light source 3
Default value: 0
Saved in: General.OptionsFileName
General.Light3X
¶X position of light source 3
Default value: 0.5
Saved in: General.OptionsFileName
General.Light3Y
¶Y position of light source 3
Default value: 0.3
Saved in: General.OptionsFileName
General.Light3Z
¶Z position of light source 3
Default value: 1
Saved in: General.OptionsFileName
General.Light3W
¶Divisor of the X, Y and Z coordinates of light source 3 (W=0 means infinitely far source)
Default value: 0
Saved in: General.OptionsFileName
General.Light4
¶Enable light source 4
Default value: 0
Saved in: General.OptionsFileName
General.Light4X
¶X position of light source 4
Default value: 0.5
Saved in: General.OptionsFileName
General.Light4Y
¶Y position of light source 4
Default value: 0.3
Saved in: General.OptionsFileName
General.Light4Z
¶Z position of light source 4
Default value: 1
Saved in: General.OptionsFileName
General.Light4W
¶Divisor of the X, Y and Z coordinates of light source 4 (W=0 means infinitely far source)
Default value: 0
Saved in: General.OptionsFileName
General.Light5
¶Enable light source 5
Default value: 0
Saved in: General.OptionsFileName
General.Light5X
¶X position of light source 5
Default value: 0.5
Saved in: General.OptionsFileName
General.Light5Y
¶Y position of light source 5
Default value: 0.3
Saved in: General.OptionsFileName
General.Light5Z
¶Z position of light source 5
Default value: 1
Saved in: General.OptionsFileName
General.Light5W
¶Divisor of the X, Y and Z coordinates of light source 5 (W=0 means infinitely far source)
Default value: 0
Saved in: General.OptionsFileName
General.LineWidth
¶Display width of lines (in pixels)
Default value: 1
Saved in: General.OptionsFileName
General.ManipulatorPositionX
¶Horizontal position (in pixels) of the upper left corner of the manipulator window
Default value: 650
Saved in: General.SessionFileName
General.ManipulatorPositionY
¶Vertical position (in pixels) of the upper left corner of the manipulator window
Default value: 150
Saved in: General.SessionFileName
General.MaxX
¶Maximum model coordinate along the X-axis (read-only)
Default value: 0
Saved in: -
General.MaxY
¶Maximum model coordinate along the Y-axis (read-only)
Default value: 0
Saved in: -
General.MaxZ
¶Maximum model coordinate along the Z-axis (read-only)
Default value: 0
Saved in: -
General.MenuWidth
¶Width (in pixels) of the menu tree
Default value: 200
Saved in: General.SessionFileName
General.MenuHeight
¶Height (in pixels) of the (detached) menu tree
Default value: 200
Saved in: General.SessionFileName
General.MenuPositionX
¶Horizontal position (in pixels) of the (detached) menu tree
Default value: 400
Saved in: General.SessionFileName
General.MenuPositionY
¶Vertical position (in pixels) of the (detached) menu tree
Default value: 400
Saved in: General.SessionFileName
General.MessageFontSize
¶Size of the font in the message window, in pixels (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
General.MessageHeight
¶Height (in pixels) of the message console when it is visible (should be > 0)
Default value: 300
Saved in: General.SessionFileName
General.MinX
¶Minimum model coordinate along the X-axis (read-only)
Default value: 0
Saved in: -
General.MinY
¶Minimum model coordinate along the Y-axis (read-only)
Default value: 0
Saved in: -
General.MinZ
¶Minimum model coordinate along the Z-axis (read-only)
Default value: 0
Saved in: -
General.MouseHoverMeshes
¶Enable mouse hover on meshes
Default value: 0
Saved in: General.OptionsFileName
General.MouseSelection
¶Enable mouse selection
Default value: 1
Saved in: General.OptionsFileName
General.MouseInvertZoom
¶Invert mouse wheel zoom direction
Default value: 0
Saved in: General.OptionsFileName
General.NativeFileChooser
¶Use the native file chooser?
Default value: 1
Saved in: General.SessionFileName
General.NonModalWindows
¶Force all control windows to be on top of the graphic window ("non-modal")
Default value: 1
Saved in: General.SessionFileName
General.NoPopup
¶Disable interactive dialog windows in scripts (and use default values instead)
Default value: 0
Saved in: General.OptionsFileName
General.NumThreads
¶Set (maximum) number of threads (0: use system default, i.e. OMP_NUM_THREADS)
Default value: 1
Saved in: General.OptionsFileName
General.OptionsPositionX
¶Horizontal position (in pixels) of the upper left corner of the option window
Default value: 650
Saved in: General.SessionFileName
General.OptionsPositionY
¶Vertical position (in pixels) of the upper left corner of the option window
Default value: 150
Saved in: General.SessionFileName
General.Orthographic
¶Orthographic projection mode (0: perspective projection)
Default value: 1
Saved in: General.OptionsFileName
General.PluginPositionX
¶Horizontal position (in pixels) of the upper left corner of the plugin window
Default value: 650
Saved in: General.SessionFileName
General.PluginPositionY
¶Vertical position (in pixels) of the upper left corner of the plugin window
Default value: 550
Saved in: General.SessionFileName
General.PluginHeight
¶Height (in pixels) of the plugin window
Default value: 320
Saved in: General.SessionFileName
General.PluginWidth
¶Width (in pixels) of the plugin window
Default value: 420
Saved in: General.SessionFileName
General.PointSize
¶Display size of points (in pixels)
Default value: 3
Saved in: General.OptionsFileName
General.PolygonOffsetAlwaysOn
¶Always apply polygon offset, instead of trying to detect when it is required
Default value: 0
Saved in: General.OptionsFileName
General.PolygonOffsetFactor
¶Polygon offset factor (offset = factor * DZ + r * units)
Default value: 0.5
Saved in: General.OptionsFileName
General.PolygonOffsetUnits
¶Polygon offset units (offset = factor * DZ + r * units)
Default value: 1
Saved in: General.OptionsFileName
General.ProgressMeterStep
¶Increment (in percent) of the progress meter bar
Default value: 10
Saved in: General.OptionsFileName
General.QuadricSubdivisions
¶Number of subdivisions used to draw points or lines as spheres or cylinders
Default value: 6
Saved in: General.OptionsFileName
General.RotationX
¶First Euler angle (used if Trackball=0)
Default value: 0
Saved in: -
General.RotationY
¶Second Euler angle (used if Trackball=0)
Default value: 0
Saved in: -
General.RotationZ
¶Third Euler angle (used if Trackball=0)
Default value: 0
Saved in: -
General.RotationCenterGravity
¶Rotate around the (pseudo) center of mass instead of (RotationCenterX, RotationCenterY, RotationCenterZ)
Default value: 1
Saved in: General.OptionsFileName
General.RotationCenterX
¶X coordinate of the center of rotation
Default value: 0
Saved in: -
General.RotationCenterY
¶Y coordinate of the center of rotation
Default value: 0
Saved in: -
General.RotationCenterZ
¶Z coordinate of the center of rotation
Default value: 0
Saved in: -
General.SaveOptions
¶Automatically save current options in General.OptionsFileName (1) or per model (2)when the graphical user interface is closed?
Default value: 0
Saved in: General.SessionFileName
General.SaveSession
¶Automatically save session specific information in General.SessionFileName when the graphical user interface is closed?
Default value: 1
Saved in: General.SessionFileName
General.ScaleX
¶X-axis scale factor
Default value: 1
Saved in: -
General.ScaleY
¶Y-axis scale factor
Default value: 1
Saved in: -
General.ScaleZ
¶Z-axis scale factor
Default value: 1
Saved in: -
General.Shininess
¶Material shininess
Default value: 0.4
Saved in: General.OptionsFileName
General.ShininessExponent
¶Material shininess exponent (between 0 and 128)
Default value: 40
Saved in: General.OptionsFileName
General.ShowModuleMenu
¶Show the standard Gmsh menu in the tree
Default value: 1
Saved in: General.OptionsFileName
General.ShowOptionsOnStartup
¶Show option window on startup
Default value: 0
Saved in: General.OptionsFileName
General.ShowMessagesOnStartup
¶Show message window on startup
Default value: 0
Saved in: General.OptionsFileName
General.SmallAxes
¶Display the small axes
Default value: 1
Saved in: General.OptionsFileName
General.SmallAxesPositionX
¶X position (in pixels) of small axes (< 0: measure from right window edge; >= 1e5: centered)
Default value: -60
Saved in: General.OptionsFileName
General.SmallAxesPositionY
¶Y position (in pixels) of small axes (< 0: measure from bottom window edge; >= 1e5: centered)
Default value: -40
Saved in: General.OptionsFileName
General.SmallAxesSize
¶Size (in pixels) of small axes
Default value: 30
Saved in: General.OptionsFileName
General.StatisticsPositionX
¶Horizontal position (in pixels) of the upper left corner of the statistic window
Default value: 650
Saved in: General.SessionFileName
General.StatisticsPositionY
¶Vertical position (in pixels) of the upper left corner of the statistic window
Default value: 150
Saved in: General.SessionFileName
General.Stereo
¶Use stereo rendering
Default value: 0
Saved in: General.OptionsFileName
General.SystemMenuBar
¶Use the system menu bar on Mac OS X?
Default value: 1
Saved in: General.SessionFileName
General.Terminal
¶Should information be printed on the terminal (if available)?
Default value: 0
Saved in: General.OptionsFileName
General.Tooltips
¶Show tooltips in the user interface
Default value: 1
Saved in: General.OptionsFileName
General.Trackball
¶Use trackball rotation mode
Default value: 1
Saved in: General.OptionsFileName
General.TrackballHyperbolicSheet
¶Use hyperbolic sheet away from trackball center for z-rotations
Default value: 1
Saved in: General.OptionsFileName
General.TrackballQuaternion0
¶First trackball quaternion component (used if General.Trackball=1)
Default value: 0
Saved in: -
General.TrackballQuaternion1
¶Second trackball quaternion component (used if General.Trackball=1)
Default value: 0
Saved in: -
General.TrackballQuaternion2
¶Third trackball quaternion component (used if General.Trackball=1)
Default value: 0
Saved in: -
General.TrackballQuaternion3
¶Fourth trackball quaternion component (used if General.Trackball=1)
Default value: 1
Saved in: -
General.TranslationX
¶X-axis translation (in model units)
Default value: 0
Saved in: -
General.TranslationY
¶Y-axis translation (in model units)
Default value: 0
Saved in: -
General.TranslationZ
¶Z-axis translation (in model units)
Default value: 0
Saved in: -
General.VectorType
¶Default vector display type (for normals, etc.)
Default value: 4
Saved in: General.OptionsFileName
General.Verbosity
¶Level of information printed on the terminal and the message console (0: silent except for fatal errors, 1: +errors, 2: +warnings, 3: +direct, 4: +information, 5: +status, 99: +debug)
Default value: 5
Saved in: General.OptionsFileName
General.VisibilityPositionX
¶Horizontal position (in pixels) of the upper left corner of the visibility window
Default value: 650
Saved in: General.SessionFileName
General.VisibilityPositionY
¶Vertical position (in pixels) of the upper left corner of the visibility window
Default value: 150
Saved in: General.SessionFileName
General.ZoomFactor
¶Middle mouse button zoom acceleration factor
Default value: 4
Saved in: General.OptionsFileName
General.Color.Background
¶Background color
Default value: {255,255,255}
Saved in: General.OptionsFileName
General.Color.BackgroundGradient
¶Background gradient color
Default value: {208,215,255}
Saved in: General.OptionsFileName
General.Color.Foreground
¶Foreground color
Default value: {85,85,85}
Saved in: General.OptionsFileName
General.Color.Text
¶Text color
Default value: {0,0,0}
Saved in: General.OptionsFileName
General.Color.Axes
¶Axes color
Default value: {0,0,0}
Saved in: General.OptionsFileName
General.Color.SmallAxes
¶Small axes color
Default value: {0,0,0}
Saved in: General.OptionsFileName
General.Color.AmbientLight
¶Ambient light color
Default value: {25,25,25}
Saved in: General.OptionsFileName
General.Color.DiffuseLight
¶Diffuse light color
Default value: {255,255,255}
Saved in: General.OptionsFileName
General.Color.SpecularLight
¶Specular light color
Default value: {255,255,255}
Saved in: General.OptionsFileName
Print.ParameterCommand
¶Command parsed when the print parameter is changed
Default value: "Mesh.Clip=1; View.Clip=1; General.ClipWholeElements=1; General.Clip0D=Print.Parameter; SetChanged;"
Saved in: General.OptionsFileName
Print.Parameter
¶Current value of the print parameter
Default value: 0
Saved in: General.OptionsFileName
Print.ParameterFirst
¶First value of print parameter in loop
Default value: -1
Saved in: General.OptionsFileName
Print.ParameterLast
¶Last value of print parameter in loop
Default value: 1
Saved in: General.OptionsFileName
Print.ParameterSteps
¶Number of steps in loop over print parameter
Default value: 10
Saved in: General.OptionsFileName
Print.Background
¶Print background (gradient and image)?
Default value: 0
Saved in: General.OptionsFileName
Print.CompositeWindows
¶Composite all window tiles in the same output image (for bitmap output only)
Default value: 0
Saved in: General.OptionsFileName
Print.DeleteTemporaryFiles
¶Delete temporary files used during printing
Default value: 1
Saved in: General.OptionsFileName
Print.EpsBestRoot
¶Try to minimize primitive splitting in BSP tree sorted PostScript/PDF output
Default value: 1
Saved in: General.OptionsFileName
Print.EpsCompress
¶Compress PostScript/PDF output using zlib
Default value: 0
Saved in: General.OptionsFileName
Print.EpsLineWidthFactor
¶Width factor for lines in PostScript/PDF output
Default value: 1
Saved in: General.OptionsFileName
Print.EpsOcclusionCulling
¶Cull occluded primitives (to reduce PostScript/PDF file size)
Default value: 1
Saved in: General.OptionsFileName
Print.EpsPointSizeFactor
¶Size factor for points in PostScript/PDF output
Default value: 1
Saved in: General.OptionsFileName
Print.EpsPS3Shading
¶Enable PostScript Level 3 shading
Default value: 0
Saved in: General.OptionsFileName
Print.EpsQuality
¶PostScript/PDF quality (0: bitmap, 1: vector (simple sort), 2: vector (accurate sort), 3: vector (unsorted)
Default value: 1
Saved in: General.OptionsFileName
Print.Format
¶File format (10: automatic)
Default value: 10
Saved in: General.OptionsFileName
Print.GeoLabels
¶Save labels in unrolled Gmsh geometries
Default value: 1
Saved in: General.OptionsFileName
Print.GeoOnlyPhysicals
¶Only save entities that belong to physical groups
Default value: 0
Saved in: General.OptionsFileName
Print.GifDither
¶Apply dithering to GIF output
Default value: 0
Saved in: General.OptionsFileName
Print.GifInterlace
¶Interlace GIF output
Default value: 0
Saved in: General.OptionsFileName
Print.GifSort
¶Sort the colormap in GIF output
Default value: 1
Saved in: General.OptionsFileName
Print.GifTransparent
¶Output transparent GIF image
Default value: 0
Saved in: General.OptionsFileName
Print.Height
¶Height of printed image; use (possibly scaled) current height if < 0
Default value: -1
Saved in: General.OptionsFileName
Print.JpegQuality
¶JPEG quality (between 1 and 100)
Default value: 100
Saved in: General.OptionsFileName
Print.JpegSmoothing
¶JPEG smoothing (between 0 and 100)
Default value: 0
Saved in: General.OptionsFileName
Print.PgfTwoDim
¶Output PGF format for two dimensions. Mostly irrelevant if ‘PgfExportAxis=0‘. Default ‘1‘ (yes).
Default value: 1
Saved in: General.OptionsFileName
Print.PgfExportAxis
¶Include axis in export pgf code (not in the png). Default ‘0‘ (no).
Default value: 0
Saved in: General.OptionsFileName
Print.PgfHorizontalBar
¶Use a horizontal color bar in the pgf output. Default ‘0‘ (no).
Default value: 0
Saved in: General.OptionsFileName
Print.PostElementary
¶Save elementary region tags in mesh statistics exported as post-processing views
Default value: 1
Saved in: General.OptionsFileName
Print.PostElement
¶Save element tags in mesh statistics exported as post-processing views
Default value: 0
Saved in: General.OptionsFileName
Print.PostGamma
¶Save Gamma quality measure in mesh statistics exported as post-processing views
Default value: 0
Saved in: General.OptionsFileName
Print.PostEta
¶Save Eta quality measure in mesh statistics exported as post-processing views
Default value: 0
Saved in: General.OptionsFileName
Print.PostSICN
¶Save SICN (signed inverse condition number) quality measure in mesh statistics exported as post-processing views
Default value: 0
Saved in: General.OptionsFileName
Print.PostSIGE
¶Save SIGE (signed inverse gradient error) quality measure in mesh statistics exported as post-processing views
Default value: 0
Saved in: General.OptionsFileName
Print.PostDisto
¶Save Disto quality measure in mesh statistics exported as post-processing views
Default value: 0
Saved in: General.OptionsFileName
Print.TexAsEquation
¶Print all TeX strings as equations
Default value: 0
Saved in: General.OptionsFileName
Print.TexForceFontSize
¶Force font size of TeX strings to fontsize in the graphic window
Default value: 0
Saved in: General.OptionsFileName
Print.TexWidthInMm
¶Width of tex graphics in mm (use 0 for the natural width inferred from the image width in pixels)
Default value: 150
Saved in: General.OptionsFileName
Print.Text
¶Print text strings?
Default value: 1
Saved in: General.OptionsFileName
Print.X3dCompatibility
¶Produce highly compatible X3D output (no scale bar)
Default value: 0
Saved in: General.OptionsFileName
Print.X3dPrecision
¶Precision of X3D output
Default value: 1e-09
Saved in: General.OptionsFileName
Print.X3dRemoveInnerBorders
¶Remove inner borders in X3D output
Default value: 0
Saved in: General.OptionsFileName
Print.X3dTransparency
¶Transparency for X3D output
Default value: 0
Saved in: General.OptionsFileName
Print.X3dSurfaces
¶Save surfaces in CAD X3D output (0: no, 1: yes in a single X3D object,2: one X3D object per geometrical surface, 3: one X3D object perphysical surface)
Default value: 1
Saved in: General.OptionsFileName
Print.X3dEdges
¶Save edges in CAD X3D output (0: no, 1: yes in a single X3D object,2: one X3D object per geometrical edge, 3: one X3D object perphysical edge)
Default value: 0
Saved in: General.OptionsFileName
Print.X3dVertices
¶Save vertices in CAD X3D output (0: no, 1: yes)
Default value: 0
Saved in: General.OptionsFileName
Print.Width
¶Width of printed image; use (possibly scaled) current width if < 0)
Default value: -1
Saved in: General.OptionsFileName
Next: Mesh options list, Previous: General options list, Up: Options [Contents][Index]
Geometry.DoubleClickedPointCommand
¶Command parsed when double-clicking on a point, or ’ONELAB’ to edit associated ONELAB parameters
Default value: "ONELAB"
Saved in: General.OptionsFileName
Geometry.DoubleClickedCurveCommand
¶Command parsed when double-clicking on a curve, or ’ONELAB’ to edit associated ONELAB parameters
Default value: "ONELAB"
Saved in: General.OptionsFileName
Geometry.DoubleClickedSurfaceCommand
¶Command parsed when double-clicking on a surface, or ’ONELAB’ to edit associated ONELAB parameters
Default value: "ONELAB"
Saved in: General.OptionsFileName
Geometry.DoubleClickedVolumeCommand
¶Command parsed when double-clicking on a volume, or ’ONELAB’ to edit associated ONELAB parameters
Default value: "ONELAB"
Saved in: General.OptionsFileName
Geometry.OCCTargetUnit
¶Length unit to which coordinates from STEP and IGES files are converted to when imported by OpenCASCADE, e.g. ’M’ for meters (leave empty to use OpenCASCADE default bahavior)
Default value: ""
Saved in: General.OptionsFileName
Geometry.AutoCoherence
¶Should all duplicate entities be automatically removed with the built-in geometry kernel? If Geometry.AutoCoherence = 2, also remove degenerate entities. The option has no effect with the OpenCASCADE kernel
Default value: 1
Saved in: General.OptionsFileName
Geometry.Clip
¶Enable clipping planes? (Plane[i]=2^i, i=0,...,5)
Default value: 0
Saved in: -
Geometry.CopyMeshingMethod
¶Copy meshing method (unstructured or transfinite) when duplicating geometrical entities with built-in geometry kernel?
Default value: 0
Saved in: General.OptionsFileName
Geometry.Curves
¶Display geometry curves?
Default value: 1
Saved in: General.OptionsFileName
Geometry.CurveLabels
¶Display curve labels?
Default value: 0
Saved in: General.OptionsFileName
Geometry.CurveSelectWidth
¶Display width of selected curves (in pixels)
Default value: 3
Saved in: General.OptionsFileName
Geometry.CurveType
¶Display curves as solid color segments (0), 3D cylinders (1) or tapered cylinders (2)
Default value: 0
Saved in: General.OptionsFileName
Geometry.CurveWidth
¶Display width of lines (in pixels)
Default value: 2
Saved in: General.OptionsFileName
Geometry.DoubleClickedEntityTag
¶Tag of last double-clicked geometrical entity
Default value: 0
Saved in: -
Geometry.ExactExtrusion
¶Use exact extrusion formula in interpolations (set to 0 to allow geometrical transformations of extruded entities)
Default value: 1
Saved in: General.OptionsFileName
Geometry.ExtrudeReturnLateralEntities
¶Add lateral entities in lists returned by extrusion commands?
Default value: 1
Saved in: General.OptionsFileName
Geometry.ExtrudeSplinePoints
¶Number of control points for splines created during extrusion
Default value: 5
Saved in: General.OptionsFileName
Geometry.HighlightOrphans
¶Highlight orphan entities (lines connected to a single surface, etc.)?
Default value: 0
Saved in: General.OptionsFileName
Geometry.LabelType
¶Type of entity label (0: description, 1: elementary entity tag, 2: physical group tag, 3: elementary name, 4: physical name)
Default value: 0
Saved in: General.OptionsFileName
Geometry.Light
¶Enable lighting for the geometry
Default value: 1
Saved in: General.OptionsFileName
Geometry.LightTwoSide
¶Light both sides of surfaces (leads to slower rendering)
Default value: 1
Saved in: General.OptionsFileName
Geometry.MatchGeomAndMesh
¶Matches geometries and meshes
Default value: 0
Saved in: General.OptionsFileName
Geometry.MatchMeshScaleFactor
¶Rescaling factor for the mesh to correspond to size of the geometry
Default value: 1
Saved in: General.OptionsFileName
Geometry.MatchMeshTolerance
¶Tolerance for matching mesh and geometry
Default value: 1e-06
Saved in: General.OptionsFileName
Geometry.Normals
¶Display size of normal vectors (in pixels)
Default value: 0
Saved in: General.OptionsFileName
Geometry.NumSubEdges
¶Number of edge subdivisions between control points when displaying curves
Default value: 40
Saved in: General.OptionsFileName
Geometry.OCCAutoFix
¶Automatically fix orientation of wires, faces, shells and volumes when creating new entities with the OpenCASCADE kernel
Default value: 1
Saved in: General.OptionsFileName
Geometry.OCCBooleanPreserveNumbering
¶Try to preserve the numbering of entities through OpenCASCADE boolean operations
Default value: 1
Saved in: General.OptionsFileName
Geometry.OCCBoundsUseStl
¶Use STL mesh for computing bounds of OpenCASCADE shapes (more accurate, but slower)
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCDisableStl
¶Disable STL creation in OpenCASCADE kernel
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCFixDegenerated
¶Fix degenerated edges/faces when importing STEP, IGES and BRep models with the OpenCASCADE kernel
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCFixSmallEdges
¶Fix small edges when importing STEP, IGES and BRep models with the OpenCASCADE kernel
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCFixSmallFaces
¶Fix small faces when importing STEP, IGES and BRep models with the OpenCASCADE kernel
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCImportLabels
¶Import labels and colors when importing STEP models with the OpenCASCADE kernel
Default value: 1
Saved in: General.OptionsFileName
Geometry.OCCMakeSolids
¶Fix shells and make solids when importing STEP, IGES and BRep models with the OpenCASCADE kernel
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCParallel
¶Use multi-threaded OpenCASCADE boolean operators
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCScaling
¶Scale STEP, IGES and BRep models by the given factor when importing them with the OpenCASCADE kernel
Default value: 1
Saved in: General.OptionsFileName
Geometry.OCCSewFaces
¶Sew faces when importing STEP, IGES and BRep models with the OpenCASCADE kernel
Default value: 0
Saved in: General.OptionsFileName
Geometry.OCCThruSectionsDegree
¶Maximum degree of surfaces generated by thrusections with the OpenCASCADE kernel, if not explicitely specified (default OCC value if negative)
Default value: -1
Saved in: General.OptionsFileName
Geometry.OCCUnionUnify
¶Try to unify faces and edges (remove internal seams) which lie on the same geometry after performing a boolean union with the OpenCASCADE kernel
Default value: 1
Saved in: General.OptionsFileName
Geometry.OCCUseGenericClosestPoint
¶Use generic algrithm to compute point projections in the OpenCASCADE kernel (less robust, but significally faster in some configurations)
Default value: 0
Saved in: General.OptionsFileName
Geometry.OffsetX
¶Model display offset along X-axis (in model coordinates)
Default value: 0
Saved in: -
Geometry.OffsetY
¶Model display offset along Y-axis (in model coordinates)
Default value: 0
Saved in: -
Geometry.OffsetZ
¶Model display offset along Z-axis (in model coordinates)
Default value: 0
Saved in: -
Geometry.OldCircle
¶Use old circle description (compatibility option for old Gmsh geometries)
Default value: 0
Saved in: General.OptionsFileName
Geometry.OldRuledSurface
¶Use old 3-sided ruled surface interpolation (compatibility option for old Gmsh geometries)
Default value: 0
Saved in: General.OptionsFileName
Geometry.OldNewReg
¶Use old newreg definition for geometrical transformations (compatibility option for old Gmsh geometries)
Default value: 1
Saved in: General.OptionsFileName
Geometry.Points
¶Display geometry points?
Default value: 1
Saved in: General.OptionsFileName
Geometry.PointLabels
¶Display points labels?
Default value: 0
Saved in: General.OptionsFileName
Geometry.PointSelectSize
¶Display size of selected points (in pixels)
Default value: 6
Saved in: General.OptionsFileName
Geometry.PointSize
¶Display size of points (in pixels)
Default value: 4
Saved in: General.OptionsFileName
Geometry.PointType
¶Display points as solid color dots (0) or 3D spheres (1)
Default value: 0
Saved in: General.OptionsFileName
Geometry.ReparamOnFaceRobust
¶Use projection for reparametrization of a point classified on GEdge on a GFace
Default value: 0
Saved in: General.OptionsFileName
Geometry.ScalingFactor
¶Global geometry scaling factor
Default value: 1
Saved in: General.OptionsFileName
Geometry.OrientedPhysicals
¶Use sign of elementary entity in physical definition as orientation indicator
Default value: 1
Saved in: General.OptionsFileName
Geometry.SnapX
¶Snapping grid spacing along the X-axis
Default value: 0.1
Saved in: General.OptionsFileName
Geometry.SnapY
¶Snapping grid spacing along the Y-axis
Default value: 0.1
Saved in: General.OptionsFileName
Geometry.SnapZ
¶Snapping grid spacing along the Z-axis
Default value: 0.1
Saved in: General.OptionsFileName
Geometry.Surfaces
¶Display geometry surfaces?
Default value: 0
Saved in: General.OptionsFileName
Geometry.SurfaceLabels
¶Display surface labels?
Default value: 0
Saved in: General.OptionsFileName
Geometry.SurfaceType
¶Surface display type (0: cross, 1: wireframe, 2: solid). Wireframe and solid are not available with the built-in geometry kernel.
Default value: 0
Saved in: General.OptionsFileName
Geometry.Tangents
¶Display size of tangent vectors (in pixels)
Default value: 0
Saved in: General.OptionsFileName
Geometry.Tolerance
¶Geometrical tolerance
Default value: 1e-08
Saved in: General.OptionsFileName
Geometry.ToleranceBoolean
¶Geometrical tolerance for boolean operations
Default value: 0
Saved in: General.OptionsFileName
Geometry.Transform
¶Transform model display coordinates (0: no, 1: scale)
Default value: 0
Saved in: -
Geometry.TransformXX
¶Element (1,1) of the 3x3 model display transformation matrix
Default value: 1
Saved in: -
Geometry.TransformXY
¶Element (1,2) of the 3x3 model display transformation matrix
Default value: 0
Saved in: -
Geometry.TransformXZ
¶Element (1,3) of the 3x3 model display transformation matrix
Default value: 0
Saved in: -
Geometry.TransformYX
¶Element (2,1) of the 3x3 model display transformation matrix
Default value: 0
Saved in: -
Geometry.TransformYY
¶Element (2,2) of the 3x3 model display transformation matrix
Default value: 1
Saved in: -
Geometry.TransformYZ
¶Element (2,3) of the 3x3 model display transformation matrix
Default value: 0
Saved in: -
Geometry.TransformZX
¶Element (3,1) of the 3x3 model display transformation matrix
Default value: 0
Saved in: -
Geometry.TransformZY
¶Element (3,2) of the 3x3 model display transformation matrix
Default value: 0
Saved in: -
Geometry.TransformZZ
¶Element (3,3) of the 3x3 model display transformation matrix
Default value: 1
Saved in: -
Geometry.Volumes
¶Display geometry volumes?
Default value: 0
Saved in: General.OptionsFileName
Geometry.VolumeLabels
¶Display volume labels?
Default value: 0
Saved in: General.OptionsFileName
Geometry.Color.Points
¶Normal geometry point color
Default value: {90,90,90}
Saved in: General.OptionsFileName
Geometry.Color.Curves
¶Normal geometry curve color
Default value: {0,0,255}
Saved in: General.OptionsFileName
Geometry.Color.Surfaces
¶Normal geometry surface color
Default value: {128,128,128}
Saved in: General.OptionsFileName
Geometry.Color.Volumes
¶Normal geometry volume color
Default value: {255,255,0}
Saved in: General.OptionsFileName
Geometry.Color.Selection
¶Selected geometry color
Default value: {255,0,0}
Saved in: General.OptionsFileName
Geometry.Color.HighlightZero
¶Highlight 0 color
Default value: {255,0,0}
Saved in: General.OptionsFileName
Geometry.Color.HighlightOne
¶Highlight 1 color
Default value: {255,150,0}
Saved in: General.OptionsFileName
Geometry.Color.HighlightTwo
¶Highlight 2 color
Default value: {255,255,0}
Saved in: General.OptionsFileName
Geometry.Color.Tangents
¶Tangent geometry vectors color
Default value: {255,255,0}
Saved in: General.OptionsFileName
Geometry.Color.Normals
¶Normal geometry vectors color
Default value: {255,0,0}
Saved in: General.OptionsFileName
Geometry.Color.Projection
¶Projection surface color
Default value: {0,255,0}
Saved in: General.OptionsFileName
Next: Solver options list, Previous: Geometry options list, Up: Options [Contents][Index]
Mesh.Algorithm
¶2D mesh algorithm (1: MeshAdapt, 2: Automatic, 3: Initial mesh only, 5: Delaunay, 6: Frontal-Delaunay, 7: BAMG, 8: Frontal-Delaunay for Quads, 9: Packing of Parallelograms)
Default value: 6
Saved in: General.OptionsFileName
Mesh.Algorithm3D
¶3D mesh algorithm (1: Delaunay, 3: Initial mesh only, 4: Frontal, 7: MMG3D, 9: R-tree, 10: HXT)
Default value: 1
Saved in: General.OptionsFileName
Mesh.AlgorithmSwitchOnFailure
¶Switch meshing algorithm on failure? (Currently only for 2D Delaunay-based algorithms, switching to MeshAdapt)
Default value: 1
Saved in: General.OptionsFileName
Mesh.AngleSmoothNormals
¶Threshold angle below which normals are not smoothed
Default value: 30
Saved in: General.OptionsFileName
Mesh.AngleToleranceFacetOverlap
¶Consider connected facets as overlapping when the dihedral angle between the facets is smaller than the user’s defined tolerance (in degrees)
Default value: 0.1
Saved in: General.OptionsFileName
Mesh.AnisoMax
¶Maximum anisotropy of the mesh
Default value: 1e+33
Saved in: General.OptionsFileName
Mesh.AllowSwapAngle
¶Threshold angle (in degrees) between faces normals under which we allow an edge swap
Default value: 10
Saved in: General.OptionsFileName
Mesh.BdfFieldFormat
¶Field format for Nastran BDF files (0: free, 1: small, 2: large)
Default value: 1
Saved in: General.OptionsFileName
Mesh.Binary
¶Write mesh files in binary format (if possible)
Default value: 0
Saved in: General.OptionsFileName
Mesh.BoundaryLayerFanElements
¶Number of elements (per Pi radians) for 2D boundary layer fans
Default value: 5
Saved in: General.OptionsFileName
Mesh.CgnsImportOrder
¶Order of the mesh to be created by coarsening CGNS structured zones (1 to 4)
Default value: 1
Saved in: General.OptionsFileName
Mesh.CgnsImportIgnoreBC
¶Ignore information in ZoneBC structures when reading a CGNS file
Default value: 0
Saved in: General.OptionsFileName
Mesh.CgnsImportIgnoreSolution
¶Ignore solution when reading a CGNS file
Default value: 0
Saved in: General.OptionsFileName
Mesh.CgnsConstructTopology
¶Reconstruct the model topology (BREP) after reading a CGNS file
Default value: 0
Saved in: General.OptionsFileName
Mesh.CgnsExportCPEX0045
¶Use the CPEX0045 convention when exporting a high-order mesh to CGNS
Default value: 0
Saved in: General.OptionsFileName
Mesh.CgnsExportStructured
¶Export transfinite meshes as structured CGNS grids
Default value: 0
Saved in: General.OptionsFileName
Mesh.Clip
¶Enable clipping planes? (Plane[i]=2^i, i=0,...,5)
Default value: 0
Saved in: -
Mesh.ColorCarousel
¶Mesh coloring (0: by element type, 1: by elementary entity, 2: by physical group, 3: by mesh partition)
Default value: 1
Saved in: General.OptionsFileName
Mesh.CompoundClassify
¶How are surface mesh elements classified on compounds? (0: on the new discrete surface, 1: on the original geometrical surfaces - incompatible with e.g. high-order meshing)
Default value: 1
Saved in: General.OptionsFileName
Mesh.CompoundMeshSizeFactor
¶Mesh size factor applied to compound parts
Default value: 0.5
Saved in: General.OptionsFileName
Mesh.CpuTime
¶CPU time (in seconds) for the generation of the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.CreateTopologyMsh2
¶Attempt to (re)create the model topology when reading MSH2 files
Default value: 0
Saved in: General.OptionsFileName
Mesh.DrawSkinOnly
¶Draw only the skin of 3D meshes?
Default value: 0
Saved in: General.OptionsFileName
Mesh.Dual
¶Display the dual mesh obtained by barycentric subdivision
Default value: 0
Saved in: General.OptionsFileName
Mesh.ElementOrder
¶Element order (1: first order elements)
Default value: 1
Saved in: General.OptionsFileName
Mesh.Explode
¶Element shrinking factor (between 0 and 1)
Default value: 1
Saved in: General.OptionsFileName
Mesh.FirstElementTag
¶First tag (>= 1) of mesh elements
Default value: 1
Saved in: General.OptionsFileName
Mesh.FirstNodeTag
¶First tag (>= 1) of mesh nodes
Default value: 1
Saved in: General.OptionsFileName
Mesh.FlexibleTransfinite
¶Allow transfinite constraints to be modified for recombination (e.g. Blossom) or by global mesh size factor
Default value: 0
Saved in: General.OptionsFileName
Mesh.Format
¶Mesh output format (1: msh, 2: unv, 10: auto, 16: vtk, 19: vrml, 21: mail, 26: pos stat, 27: stl, 28: p3d, 30: mesh, 31: bdf, 32: cgns, 33: med, 34: diff, 38: ir3, 39: inp, 40: ply2, 41: celum, 42: su2, 47: tochnog, 49: neu, 50: matlab)
Default value: 10
Saved in: General.OptionsFileName
Mesh.Hexahedra
¶Display mesh hexahedra?
Default value: 1
Saved in: General.OptionsFileName
Mesh.HighOrderDistCAD
¶Try to optimize distance to CAD in high-order optimizer?
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderIterMax
¶Maximum number of iterations in high-order optimization pass
Default value: 100
Saved in: General.OptionsFileName
Mesh.HighOrderNumLayers
¶Number of layers around a problematic element to consider for high-order optimization, or number of element layers to consider in the boundary layer mesh for high-order fast curving
Default value: 6
Saved in: General.OptionsFileName
Mesh.HighOrderOptimize
¶Optimize high-order meshes? (0: none, 1: optimization, 2: elastic+optimization, 3: elastic, 4: fast curving)
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderPassMax
¶Maximum number of high-order optimization passes (moving barrier)
Default value: 25
Saved in: General.OptionsFileName
Mesh.HighOrderPeriodic
¶Force location of nodes for periodic meshes using periodicity transform (0: assume identical parametrisations, 1: invert parametrisations, 2: compute closest point
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderPoissonRatio
¶Poisson ratio of the material used in the elastic smoother for high-order meshes (between -1.0 and 0.5, excluded)
Default value: 0.33
Saved in: General.OptionsFileName
Mesh.HighOrderSavePeriodic
¶Save high-order nodes in periodic section of MSH files?
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderPrimSurfMesh
¶Try to fix flipped surface mesh elements in high-order optimizer?
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderThresholdMin
¶Minimum threshold for high-order element optimization
Default value: 0.1
Saved in: General.OptionsFileName
Mesh.HighOrderThresholdMax
¶Maximum threshold for high-order element optimization
Default value: 2
Saved in: General.OptionsFileName
Mesh.HighOrderFastCurvingNewAlgo
¶Curve boundary layer with new "fast curving" algorithm (experimental)
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderCurveOuterBL
¶Curve also the outer surface of the boundary layer in the fast curving algorithm (0 = do not curve, 1 = curve according to boundary, 2 = curve without breaking outer elements)
Default value: 0
Saved in: General.OptionsFileName
Mesh.HighOrderMaxRho
¶Maximum min/max ratio of edge/face size for the detection of BL element columns in the fast curving algorithm
Default value: 0.3
Saved in: General.OptionsFileName
Mesh.HighOrderMaxAngle
¶Maximum angle between layers of BL elements for the detection of columns in the fast curving algorithm
Default value: 0.174533
Saved in: General.OptionsFileName
Mesh.HighOrderMaxInnerAngle
¶Maximum angle between edges/faces within layers of BL triangles/tets for the detection of columns in the fast curving algorithm
Default value: 0.523599
Saved in: General.OptionsFileName
Mesh.IgnoreParametrization
¶Skip parametrization section when reading meshes in the MSH4 format.
Default value: 0
Saved in: General.OptionsFileName
Mesh.IgnorePeriodicity
¶Skip periodic node section and skip periodic boundary alignement step when reading meshes in the MSH2 format.
Default value: 1
Saved in: General.OptionsFileName
Mesh.LabelSampling
¶Label sampling rate (display one label every ‘LabelSampling’ elements)
Default value: 1
Saved in: General.OptionsFileName
Mesh.LabelType
¶Type of element label (0: node/element tag, 1: elementary entity tag, 2: physical entity tag, 3: partition, 4: coordinates)
Default value: 0
Saved in: General.OptionsFileName
Mesh.LcIntegrationPrecision
¶Accuracy of evaluation of the LC field for 1D mesh generation
Default value: 1e-09
Saved in: General.OptionsFileName
Mesh.Light
¶Enable lighting for the mesh
Default value: 1
Saved in: General.OptionsFileName
Mesh.LightLines
¶Enable lighting for mesh edges (0: no, 1: surfaces, 2: surfaces+volumes
Default value: 2
Saved in: General.OptionsFileName
Mesh.LightTwoSide
¶Light both sides of surfaces (leads to slower rendering)
Default value: 1
Saved in: General.OptionsFileName
Mesh.Lines
¶Display mesh lines (1D elements)?
Default value: 0
Saved in: General.OptionsFileName
Mesh.LineLabels
¶Display mesh line labels?
Default value: 0
Saved in: General.OptionsFileName
Mesh.LineWidth
¶Display width of mesh lines (in pixels)
Default value: 1
Saved in: General.OptionsFileName
Mesh.MaxIterDelaunay3D
¶Maximum number of point insertion iterations in 3D Delaunay mesher (0: unlimited)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MaxNumThreads1D
¶Maximum number of threads for 1D meshing (0: use default)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MaxNumThreads2D
¶Maximum number of threads for 2D meshing (0: use default)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MaxNumThreads3D
¶Maximum number of threads for 3D meshing (0: use default)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MaxRetries
¶Maximum number of times meshing is retried on curves and surfaces with a pending mesh
Default value: 10
Saved in: General.OptionsFileName
Mesh.MeshOnlyVisible
¶Mesh only visible entities (experimental)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MeshOnlyEmpty
¶Mesh only entities that have no existing mesh
Default value: 0
Saved in: General.OptionsFileName
Mesh.MeshSizeExtendFromBoundary
¶Extend computation of mesh element sizes from the boundaries into the interior (for 3D Delaunay, use 1: longest or 2: shortest surface edge length)
Default value: 1
Saved in: General.OptionsFileName
Mesh.MeshSizeFactor
¶Factor applied to all mesh element sizes
Default value: 1
Saved in: General.OptionsFileName
Mesh.MeshSizeMin
¶Minimum mesh element size
Default value: 0
Saved in: General.OptionsFileName
Mesh.MeshSizeMax
¶Maximum mesh element size
Default value: 1e+22
Saved in: General.OptionsFileName
Mesh.MeshSizeFromCurvature
¶Automatically compute mesh element sizes from curvature, using the value as the target number of elements per 2 * Pi radians
Default value: 0
Saved in: General.OptionsFileName
Mesh.MeshSizeFromCurvatureIsotropic
¶Force isotropic curvature estimation when the mesh size is computed from curvature
Default value: 0
Saved in: General.OptionsFileName
Mesh.MeshSizeFromPoints
¶Compute mesh element sizes from values given at geometry points
Default value: 1
Saved in: General.OptionsFileName
Mesh.MeshSizeFromParametricPoints
¶Compute mesh element sizes from values given at geometry points defining parametric curves
Default value: 0
Saved in: General.OptionsFileName
Mesh.MetisAlgorithm
¶METIS partitioning algorithm ’ptype’ (1: Recursive, 2: K-way)
Default value: 1
Saved in: General.OptionsFileName
Mesh.MetisEdgeMatching
¶METIS edge matching type ’ctype’ (1: Random, 2: Sorted Heavy-Edge)
Default value: 2
Saved in: General.OptionsFileName
Mesh.MetisMaxLoadImbalance
¶METIS maximum load imbalance ’ufactor’ (-1: default, i.e. 30 for K-way and 1 for Recursive)
Default value: -1
Saved in: General.OptionsFileName
Mesh.MetisObjective
¶METIS objective type ’objtype’ (1: min. edge-cut, 2: min. communication volume)
Default value: 1
Saved in: General.OptionsFileName
Mesh.MetisMinConn
¶METIS minimize maximum connectivity of partitions ’minconn’ (-1: default)
Default value: -1
Saved in: General.OptionsFileName
Mesh.MetisRefinementAlgorithm
¶METIS algorithm for k-way refinement ’rtype’ (1: FM-based cut, 2: Greedy, 3: Two-sided node FM, 4: One-sided node FM)
Default value: 2
Saved in: General.OptionsFileName
Mesh.MinimumCircleNodes
¶Minimum number of nodes used to mesh circles and ellipses
Default value: 7
Saved in: General.OptionsFileName
Mesh.MinimumCurveNodes
¶Minimum number of nodes used to mesh curves other than lines, circles and ellipses
Default value: 3
Saved in: General.OptionsFileName
Mesh.MinimumElementsPerTwoPi
¶[Deprecated]
Default value: 0
Saved in: General.OptionsFileName
Mesh.MshFileVersion
¶Version of the MSH file format to use
Default value: 4.1
Saved in: General.OptionsFileName
Mesh.MedFileMinorVersion
¶Minor version of the MED file format to use (-1: use minor version of the MED library)
Default value: -1
Saved in: General.OptionsFileName
Mesh.MedImportGroupsOfNodes
¶Import groups of nodes (0: no; 1: create geometrical point for each node)?
Default value: 0
Saved in: General.OptionsFileName
Mesh.MedSingleModel
¶Import MED meshes in the current model, even if several MED mesh names exist
Default value: 0
Saved in: General.OptionsFileName
Mesh.NbHexahedra
¶Number of hexahedra in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbNodes
¶Number of nodes in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbPartitions
¶Number of partitions
Default value: 0
Saved in: General.OptionsFileName
Mesh.NbPrisms
¶Number of prisms in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbPyramids
¶Number of pyramids in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbTrihedra
¶Number of trihedra in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbQuadrangles
¶Number of quadrangles in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbTetrahedra
¶Number of tetrahedra in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NbTriangles
¶Number of triangles in the current mesh (read-only)
Default value: 0
Saved in: -
Mesh.NewtonConvergenceTestXYZ
¶Force inverse surface mapping algorithm (Newton-Raphson) to converge in real coordinates (experimental)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Nodes
¶Display mesh nodes?
Default value: 0
Saved in: General.OptionsFileName
Mesh.NodeLabels
¶Display mesh node labels?
Default value: 0
Saved in: General.OptionsFileName
Mesh.NodeSize
¶Display size of mesh nodes (in pixels)
Default value: 4
Saved in: General.OptionsFileName
Mesh.NodeType
¶Display mesh nodes as solid color dots (0) or 3D spheres (1)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Normals
¶Display size of normal vectors (in pixels)
Default value: 0
Saved in: General.OptionsFileName
Mesh.NumSubEdges
¶Number of edge subdivisions when displaying high-order elements
Default value: 2
Saved in: General.OptionsFileName
Mesh.Optimize
¶Optimize the mesh to improve the quality of tetrahedral elements
Default value: 1
Saved in: General.OptionsFileName
Mesh.OptimizeThreshold
¶Optimize tetrahedra that have a quality below ...
Default value: 0.3
Saved in: General.OptionsFileName
Mesh.OptimizeNetgen
¶Optimize the mesh using Netgen to improve the quality of tetrahedral elements
Default value: 0
Saved in: General.OptionsFileName
Mesh.PartitionHexWeight
¶Weight of hexahedral element for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionLineWeight
¶Weight of line element for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionPrismWeight
¶Weight of prismatic element (wedge) for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionPyramidWeight
¶Weight of pyramidal element for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionQuadWeight
¶Weight of quadrangle for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionTrihedronWeight
¶Weight of trihedron element for METIS load balancing (-1: automatic)
Default value: 0
Saved in: General.OptionsFileName
Mesh.PartitionTetWeight
¶Weight of tetrahedral element for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionTriWeight
¶Weight of triangle element for METIS load balancing (-1: automatic)
Default value: -1
Saved in: General.OptionsFileName
Mesh.PartitionCreateTopology
¶Create boundary representation of partitions
Default value: 1
Saved in: General.OptionsFileName
Mesh.PartitionCreatePhysicals
¶Create physical groups for partitions, based on existing physical groups
Default value: 1
Saved in: General.OptionsFileName
Mesh.PartitionCreateGhostCells
¶Create ghost cells, i.e. create for each partition a ghost entity containing elements connected to neighboring partitions by at least one node.
Default value: 0
Saved in: General.OptionsFileName
Mesh.PartitionSplitMeshFiles
¶Write one file for each mesh partition
Default value: 0
Saved in: General.OptionsFileName
Mesh.PartitionTopologyFile
¶Write a .pro file with the partition topology
Default value: 0
Saved in: General.OptionsFileName
Mesh.PartitionOldStyleMsh2
¶Write partitioned meshes in MSH2 format using old style (i.e. by not referencing new partitioned entities, except on partition boundaries), for backward compatibility
Default value: 1
Saved in: General.OptionsFileName
Mesh.PartitionConvertMsh2
¶When reading partitioned meshes in MSH2 format, create new partition entities
Default value: 1
Saved in: General.OptionsFileName
Mesh.PreserveNumberingMsh2
¶Preserve element numbering in MSH2 format (will break meshes with multiple physical groups for a single elementary entity)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Prisms
¶Display mesh prisms?
Default value: 1
Saved in: General.OptionsFileName
Mesh.Pyramids
¶Display mesh pyramids?
Default value: 1
Saved in: General.OptionsFileName
Mesh.Trihedra
¶Display mesh trihedra?
Default value: 1
Saved in: General.OptionsFileName
Mesh.Quadrangles
¶Display mesh quadrangles?
Default value: 1
Saved in: General.OptionsFileName
Mesh.QualityInf
¶Only display elements whose quality measure is greater than QualityInf
Default value: 0
Saved in: General.OptionsFileName
Mesh.QualitySup
¶Only display elements whose quality measure is smaller than QualitySup
Default value: 0
Saved in: General.OptionsFileName
Mesh.QualityType
¶Type of quality measure (0: SICN~signed inverse condition number, 1: SIGE~signed inverse gradient error, 2: gamma~vol/sum_face/max_edge, 3: Disto~minJ/maxJ
Default value: 2
Saved in: General.OptionsFileName
Mesh.RadiusInf
¶Only display elements whose longest edge is greater than RadiusInf
Default value: 0
Saved in: General.OptionsFileName
Mesh.RadiusSup
¶Only display elements whose longest edge is smaller than RadiusSup
Default value: 0
Saved in: General.OptionsFileName
Mesh.RandomFactor
¶Random factor used in the 2D meshing algorithm (should be increased if RandomFactor * size(triangle)/size(model) approaches machine accuracy)
Default value: 1e-09
Saved in: General.OptionsFileName
Mesh.RandomFactor3D
¶Random factor used in the 3D meshing algorithm
Default value: 1e-12
Saved in: General.OptionsFileName
Mesh.RandomSeed
¶Seed of pseudo-random number generator
Default value: 1
Saved in: General.OptionsFileName
Mesh.ReadGroupsOfElements
¶Read groups of elements in UNV meshes (this will discard the elementary entity tags inferred from the element section)
Default value: 1
Saved in: General.OptionsFileName
Mesh.RecombinationAlgorithm
¶Mesh recombination algorithm (0: simple, 1: blossom, 2: simple full-quad, 3: blossom full-quad)
Default value: 1
Saved in: General.OptionsFileName
Mesh.RecombineAll
¶Apply recombination algorithm to all surfaces, ignoring per-surface spec
Default value: 0
Saved in: General.OptionsFileName
Mesh.RecombineOptimizeTopology
¶Number of topological optimization passes (removal of diamonds, ...) of recombined surface meshes
Default value: 5
Saved in: General.OptionsFileName
Mesh.Recombine3DAll
¶Apply recombination3D algorithm to all volumes, ignoring per-volume spec (experimental)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Recombine3DLevel
¶3d recombination level (0: hex, 1: hex+prisms, 2: hex+prism+pyramids) (experimental)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Recombine3DConformity
¶3d recombination conformity type (0: nonconforming, 1: trihedra, 2: pyramids+trihedra, 3:pyramids+hexSplit+trihedra, 4:hexSplit+trihedra)(experimental)
Default value: 0
Saved in: General.OptionsFileName
Mesh.RefineSteps
¶Number of refinement steps in the MeshAdapt-based 2D algorithms
Default value: 10
Saved in: General.OptionsFileName
Mesh.Renumber
¶Renumber nodes and elements in a continuous sequence after mesh generation
Default value: 1
Saved in: General.OptionsFileName
Mesh.ReparamMaxTriangles
¶Maximum number of triangles in a single parametrization patch
Default value: 250000
Saved in: General.OptionsFileName
Mesh.SaveAll
¶Save all elements, even if they don’t belong to physical groups (for some mesh formats, this removes physical groups altogether)
Default value: 0
Saved in: -
Mesh.SaveElementTagType
¶Type of the element tag saved in mesh formats that don’t support saving physical or partition ids (1: elementary, 2: physical, 3: partition)
Default value: 1
Saved in: General.OptionsFileName
Mesh.SaveTopology
¶Save model topology in MSH2 output files (this is always saved in MSH3 and above)
Default value: 0
Saved in: General.OptionsFileName
Mesh.SaveParametric
¶Save parametric coordinates of nodes
Default value: 0
Saved in: General.OptionsFileName
Mesh.SaveGroupsOfElements
¶Save groups of elements for each physical group (for UNV and INP mesh format)
Default value: 1
Saved in: General.OptionsFileName
Mesh.SaveGroupsOfNodes
¶Save groups of nodes for each physical group (for UNV, INP and Tochnog mesh formats). For the INP format, a negative value will save a group of node for each entity of dimension = (-Mesh.SaveGroupsOfNodes)
Default value: 0
Saved in: General.OptionsFileName
Mesh.ScalingFactor
¶Global scaling factor applied to the saved mesh
Default value: 1
Saved in: General.OptionsFileName
Mesh.SecondOrderIncomplete
¶Create incomplete second order elements? (8-node quads, 20-node hexas, etc.)
Default value: 0
Saved in: General.OptionsFileName
Mesh.SecondOrderLinear
¶Should second order nodes (as well as nodes generated with subdivision algorithms) simply be created by linear interpolation?
Default value: 0
Saved in: General.OptionsFileName
Mesh.Smoothing
¶Number of smoothing steps applied to the final mesh
Default value: 1
Saved in: General.OptionsFileName
Mesh.SmoothCrossField
¶Apply n barycentric smoothing passes to the 3D cross field
Default value: 0
Saved in: General.OptionsFileName
Mesh.CrossFieldClosestPoint
¶Use closest point to compute 2D crossfield
Default value: 1
Saved in: General.OptionsFileName
Mesh.SmoothNormals
¶Smooth the mesh normals?
Default value: 0
Saved in: General.OptionsFileName
Mesh.SmoothRatio
¶Ratio between mesh sizes at nodes of a same edge (used in BAMG)
Default value: 1.8
Saved in: General.OptionsFileName
Mesh.StlAngularDeflection
¶Maximum angular deflection when creating STL representation of surfaces (currently only used with the OpenCASCADE kernel)
Default value: 0.35
Saved in: General.OptionsFileName
Mesh.StlLinearDeflection
¶Maximum linear deflection when creating STL representation of surfaces (currently only used with the OpenCASCADE kernel)
Default value: 0.01
Saved in: General.OptionsFileName
Mesh.StlOneSolidPerSurface
¶Create one solid per surface when exporting STL files? (0: single solid, 1: one solid per face, 2: one solid per physical surface)
Default value: 0
Saved in: General.OptionsFileName
Mesh.StlRemoveDuplicateTriangles
¶Remove duplicate triangles when importing STL files?
Default value: 0
Saved in: General.OptionsFileName
Mesh.SubdivisionAlgorithm
¶Mesh subdivision algorithm (0: none, 1: all quadrangles, 2: all hexahedra, 3: barycentric)
Default value: 0
Saved in: General.OptionsFileName
Mesh.SurfaceEdges
¶Display edges of surface mesh?
Default value: 1
Saved in: General.OptionsFileName
Mesh.SurfaceFaces
¶Display faces of surface mesh?
Default value: 0
Saved in: General.OptionsFileName
Mesh.SurfaceLabels
¶Display surface mesh element labels?
Default value: 0
Saved in: General.OptionsFileName
Mesh.SwitchElementTags
¶Invert elementary and physical tags when reading the mesh
Default value: 0
Saved in: General.OptionsFileName
Mesh.Tangents
¶Display size of tangent vectors (in pixels)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Tetrahedra
¶Display mesh tetrahedra?
Default value: 1
Saved in: General.OptionsFileName
Mesh.ToleranceEdgeLength
¶Skip a model edge in mesh generation if its length is less than user’s defined tolerance
Default value: 0
Saved in: General.OptionsFileName
Mesh.ToleranceInitialDelaunay
¶Tolerance for initial 3D Delaunay mesher
Default value: 1e-08
Saved in: General.OptionsFileName
Mesh.Triangles
¶Display mesh triangles?
Default value: 1
Saved in: General.OptionsFileName
Mesh.UnvStrictFormat
¶Use strict format specification for UNV files, with ’D’ for exponents (instead of ’E’ as used by some tools)
Default value: 1
Saved in: General.OptionsFileName
Mesh.VolumeEdges
¶Display edges of volume mesh?
Default value: 1
Saved in: General.OptionsFileName
Mesh.VolumeFaces
¶Display faces of volume mesh?
Default value: 0
Saved in: General.OptionsFileName
Mesh.VolumeLabels
¶Display volume mesh element labels?
Default value: 0
Saved in: General.OptionsFileName
Mesh.Voronoi
¶Display the voronoi diagram
Default value: 0
Saved in: General.OptionsFileName
Mesh.ZoneDefinition
¶Method for defining a zone (0: single zone, 1: by partition, 2: by physical)
Default value: 0
Saved in: General.OptionsFileName
Mesh.Color.Nodes
¶Mesh node color
Default value: {0,0,255}
Saved in: General.OptionsFileName
Mesh.Color.NodesSup
¶Second order mesh node color
Default value: {255,0,255}
Saved in: General.OptionsFileName
Mesh.Color.Lines
¶Mesh line color
Default value: {0,0,0}
Saved in: General.OptionsFileName
Mesh.Color.Triangles
¶Mesh triangle color (if Mesh.ColorCarousel=0)
Default value: {160,150,255}
Saved in: General.OptionsFileName
Mesh.Color.Quadrangles
¶Mesh quadrangle color (if Mesh.ColorCarousel=0)
Default value: {130,120,225}
Saved in: General.OptionsFileName
Mesh.Color.Tetrahedra
¶Mesh tetrahedron color (if Mesh.ColorCarousel=0)
Default value: {160,150,255}
Saved in: General.OptionsFileName
Mesh.Color.Hexahedra
¶Mesh hexahedron color (if Mesh.ColorCarousel=0)
Default value: {130,120,225}
Saved in: General.OptionsFileName
Mesh.Color.Prisms
¶Mesh prism color (if Mesh.ColorCarousel=0)
Default value: {232,210,23}
Saved in: General.OptionsFileName
Mesh.Color.Pyramids
¶Mesh pyramid color (if Mesh.ColorCarousel=0)
Default value: {217,113,38}
Saved in: General.OptionsFileName
Mesh.Color.Trihedra
¶Mesh trihedron color (if Mesh.ColorCarousel=0)
Default value: {20,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Tangents
¶Tangent mesh vector color
Default value: {255,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Normals
¶Normal mesh vector color
Default value: {255,0,0}
Saved in: General.OptionsFileName
Mesh.Color.Zero
¶Color 0 in color carousel
Default value: {255,120,0}
Saved in: General.OptionsFileName
Mesh.Color.One
¶Color 1 in color carousel
Default value: {0,255,132}
Saved in: General.OptionsFileName
Mesh.Color.Two
¶Color 2 in color carousel
Default value: {255,160,0}
Saved in: General.OptionsFileName
Mesh.Color.Three
¶Color 3 in color carousel
Default value: {0,255,192}
Saved in: General.OptionsFileName
Mesh.Color.Four
¶Color 4 in color carousel
Default value: {255,200,0}
Saved in: General.OptionsFileName
Mesh.Color.Five
¶Color 5 in color carousel
Default value: {0,216,255}
Saved in: General.OptionsFileName
Mesh.Color.Six
¶Color 6 in color carousel
Default value: {255,240,0}
Saved in: General.OptionsFileName
Mesh.Color.Seven
¶Color 7 in color carousel
Default value: {0,176,255}
Saved in: General.OptionsFileName
Mesh.Color.Eight
¶Color 8 in color carousel
Default value: {228,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Nine
¶Color 9 in color carousel
Default value: {0,116,255}
Saved in: General.OptionsFileName
Mesh.Color.Ten
¶Color 10 in color carousel
Default value: {188,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Eleven
¶Color 11 in color carousel
Default value: {0,76,255}
Saved in: General.OptionsFileName
Mesh.Color.Twelve
¶Color 12 in color carousel
Default value: {148,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Thirteen
¶Color 13 in color carousel
Default value: {24,0,255}
Saved in: General.OptionsFileName
Mesh.Color.Fourteen
¶Color 14 in color carousel
Default value: {108,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Fifteen
¶Color 15 in color carousel
Default value: {84,0,255}
Saved in: General.OptionsFileName
Mesh.Color.Sixteen
¶Color 16 in color carousel
Default value: {68,255,0}
Saved in: General.OptionsFileName
Mesh.Color.Seventeen
¶Color 17 in color carousel
Default value: {104,0,255}
Saved in: General.OptionsFileName
Mesh.Color.Eighteen
¶Color 18 in color carousel
Default value: {0,255,52}
Saved in: General.OptionsFileName
Mesh.Color.Nineteen
¶Color 19 in color carousel
Default value: {184,0,255}
Saved in: General.OptionsFileName
Next: Post-processing options list, Previous: Mesh options list, Up: Options [Contents][Index]
Solver.Executable0
¶System command to launch solver 0
Default value: ""
Saved in: General.SessionFileName
Solver.Executable1
¶System command to launch solver 1
Default value: ""
Saved in: General.SessionFileName
Solver.Executable2
¶System command to launch solver 2
Default value: ""
Saved in: General.SessionFileName
Solver.Executable3
¶System command to launch solver 3
Default value: ""
Saved in: General.SessionFileName
Solver.Executable4
¶System command to launch solver 4
Default value: ""
Saved in: General.SessionFileName
Solver.Executable5
¶System command to launch solver 5
Default value: ""
Saved in: General.SessionFileName
Solver.Executable6
¶System command to launch solver 6
Default value: ""
Saved in: General.SessionFileName
Solver.Executable7
¶System command to launch solver 7
Default value: ""
Saved in: General.SessionFileName
Solver.Executable8
¶System command to launch solver 8
Default value: ""
Saved in: General.SessionFileName
Solver.Executable9
¶System command to launch solver 9
Default value: ""
Saved in: General.SessionFileName
Solver.Name0
¶Name of solver 0
Default value: "GetDP"
Saved in: General.SessionFileName
Solver.Name1
¶Name of solver 1
Default value: ""
Saved in: General.SessionFileName
Solver.Name2
¶Name of solver 2
Default value: ""
Saved in: General.SessionFileName
Solver.Name3
¶Name of solver 3
Default value: ""
Saved in: General.SessionFileName
Solver.Name4
¶Name of solver 4
Default value: ""
Saved in: General.SessionFileName
Solver.Name5
¶Name of solver 5
Default value: ""
Saved in: General.SessionFileName
Solver.Name6
¶Name of solver 6
Default value: ""
Saved in: General.SessionFileName
Solver.Name7
¶Name of solver 7
Default value: ""
Saved in: General.SessionFileName
Solver.Name8
¶Name of solver 8
Default value: ""
Saved in: General.SessionFileName
Solver.Name9
¶Name of solver 9
Default value: ""
Saved in: General.SessionFileName
Solver.Extension0
¶File extension for solver 0
Default value: ".pro"
Saved in: General.SessionFileName
Solver.Extension1
¶File extension for solver 1
Default value: ""
Saved in: General.SessionFileName
Solver.Extension2
¶File extension for solver 2
Default value: ""
Saved in: General.SessionFileName
Solver.Extension3
¶File extension for solver 3
Default value: ""
Saved in: General.SessionFileName
Solver.Extension4
¶File extension for solver 4
Default value: ""
Saved in: General.SessionFileName
Solver.Extension5
¶File extension for solver 5
Default value: ""
Saved in: General.SessionFileName
Solver.Extension6
¶File extension for solver 6
Default value: ""
Saved in: General.SessionFileName
Solver.Extension7
¶File extension for solver 7
Default value: ""
Saved in: General.SessionFileName
Solver.Extension8
¶File extension for solver 8
Default value: ""
Saved in: General.SessionFileName
Solver.Extension9
¶File extension for solver 9
Default value: ""
Saved in: General.SessionFileName
Solver.OctaveInterpreter
¶Name of the Octave interpreter (used to run .m files)
Default value: "octave"
Saved in: General.SessionFileName
Solver.PythonInterpreter
¶Name of the Python interpreter (used to run .py files if they are not executable)
Default value: "python"
Saved in: General.SessionFileName
Solver.RemoteLogin0
¶Command to login to a remote host to launch solver 0
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin1
¶Command to login to a remote host to launch solver 1
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin2
¶Command to login to a remote host to launch solver 2
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin3
¶Command to login to a remote host to launch solver 3
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin4
¶Command to login to a remote host to launch solver 4
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin5
¶Command to login to a remote host to launch solver 5
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin6
¶Command to login to a remote host to launch solver 6
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin7
¶Command to login to a remote host to launch solver 7
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin8
¶Command to login to a remote host to launch solver 8
Default value: ""
Saved in: General.SessionFileName
Solver.RemoteLogin9
¶Command to login to a remote host to launch solver 9
Default value: ""
Saved in: General.SessionFileName
Solver.SocketName
¶Base name of socket (UNIX socket if the name does not contain a colon, TCP/IP otherwise, in the form ’host:baseport’; the actual name/port is constructed by appending the unique client id. If baseport is 0 or is not provided, the port is chosen automatically (recommended))
Default value: ".gmshsock"
Saved in: General.OptionsFileName
Solver.AlwaysListen
¶Always listen to incoming connection requests?
Default value: 0
Saved in: General.OptionsFileName
Solver.AutoArchiveOutputFiles
¶Automatically archive output files after each computation
Default value: 0
Saved in: General.OptionsFileName
Solver.AutoCheck
¶Automatically check model every time a parameter is changed
Default value: 1
Saved in: General.OptionsFileName
Solver.AutoLoadDatabase
¶Automatically load the ONELAB database when launching a solver
Default value: 0
Saved in: General.OptionsFileName
Solver.AutoSaveDatabase
¶Automatically save the ONELAB database after each computation
Default value: 1
Saved in: General.OptionsFileName
Solver.AutoMesh
¶Automatically mesh (0: never; 1: if geometry changed, but use existing mesh on disk if available; 2: if geometry changed; -1: the geometry script creates the mesh)
Default value: 2
Saved in: General.OptionsFileName
Solver.AutoMergeFile
¶Automatically merge result files
Default value: 1
Saved in: General.OptionsFileName
Solver.AutoShowViews
¶Automcatically show newly merged results (0: none; 1: all; 2: last one)
Default value: 2
Saved in: General.OptionsFileName
Solver.AutoShowLastStep
¶Automatically show the last step in newly merged results, if there are more than 2 steps
Default value: 1
Saved in: General.OptionsFileName
Solver.Plugins
¶Enable default solver plugins?
Default value: 0
Saved in: General.OptionsFileName
Solver.ShowInvisibleParameters
¶Show all parameters, even those marked invisible
Default value: 0
Saved in: General.OptionsFileName
Solver.Timeout
¶Time (in seconds) before closing the socket if no connection is happening
Default value: 5
Saved in: General.OptionsFileName
Previous: Solver options list, Up: Options [Contents][Index]
PostProcessing.DoubleClickedGraphPointCommand
¶Command parsed when double-clicking on a graph data point (e.g. Merge Sprintf(’file_%g.pos’, PostProcessing.GraphPointX);)
Default value: ""
Saved in: General.OptionsFileName
PostProcessing.GraphPointCommand
¶Synonym for ‘DoubleClickedGraphPointCommand’
Default value: ""
Saved in: General.OptionsFileName
PostProcessing.AnimationDelay
¶Delay (in seconds) between frames in automatic animation mode
Default value: 0.1
Saved in: General.OptionsFileName
PostProcessing.AnimationCycle
¶Cycle through time steps (0) or views (1) for animations
Default value: 0
Saved in: General.OptionsFileName
PostProcessing.AnimationStep
¶Step increment for animations
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.CombineRemoveOriginal
¶Remove original views after a Combine operation
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.CombineCopyOptions
¶Copy options during Combine operation
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.DoubleClickedGraphPointX
¶Abscissa of last double-clicked graph point
Default value: 0
Saved in: -
PostProcessing.DoubleClickedGraphPointY
¶Ordinate of last double-clicked graph point
Default value: 0
Saved in: -
PostProcessing.DoubleClickedView
¶Index of last double-clicked view
Default value: 0
Saved in: -
PostProcessing.ForceElementData
¶Try to force saving datasets as ElementData
Default value: 0
Saved in: General.OptionsFileName
PostProcessing.ForceNodeData
¶Try to force saving datasets as NodeData
Default value: 0
Saved in: General.OptionsFileName
PostProcessing.Format
¶Default file format for post-processing views (0: ASCII view, 1: binary view, 2: parsed view, 3: STL triangulation, 4: raw text, 5: Gmsh mesh, 6: MED file, 10: automatic)
Default value: 10
Saved in: General.OptionsFileName
PostProcessing.GraphPointX
¶Synonym for ‘DoubleClickedGraphPointX’
Default value: 0
Saved in: -
PostProcessing.GraphPointY
¶Synonym for ‘DoubleClickedGraphPointY’
Default value: 0
Saved in: -
PostProcessing.HorizontalScales
¶Display value scales horizontally
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.Link
¶Post-processing view links (0: apply next option changes to selected views, 1: force same options for all selected views)
Default value: 0
Saved in: General.OptionsFileName
PostProcessing.NbViews
¶Current number of views merged (read-only)
Default value: 0
Saved in: -
PostProcessing.Plugins
¶Enable default post-processing plugins?
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.SaveInterpolationMatrices
¶Save the interpolation matrices when exporting model-based data
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.SaveMesh
¶Save the mesh when exporting model-based data
Default value: 1
Saved in: General.OptionsFileName
PostProcessing.Smoothing
¶Apply (non-reversible) smoothing to post-processing view when merged
Default value: 0
Saved in: General.OptionsFileName
View.Attributes
¶Optional string attached to the view. If the string contains ’AlwaysVisible’, the view will not be hidden when new ones are merged.
Default value: ""
Saved in: General.OptionsFileName
View.AxesFormatX
¶Number format for X-axis (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
View.AxesFormatY
¶Number format for Y-axis (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
View.AxesFormatZ
¶Number format for Z-axis (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
View.AxesLabelX
¶X-axis label
Default value: ""
Saved in: General.OptionsFileName
View.AxesLabelY
¶Y-axis label
Default value: ""
Saved in: General.OptionsFileName
View.AxesLabelZ
¶Z-axis label
Default value: ""
Saved in: General.OptionsFileName
View.DoubleClickedCommand
¶Command parsed when double-clicking on the view
Default value: ""
Saved in: General.OptionsFileName
View.FileName
¶Default post-processing view file name
Default value: ""
Saved in: -
View.Format
¶Number format (in standard C form)
Default value: "%.3g"
Saved in: General.OptionsFileName
View.GeneralizedRaiseX
¶Generalized elevation of the view along X-axis (in model coordinates, using formula possibly containing x, y, z, s[tep], t[ime], v0, ... v8)
Default value: "v0"
Saved in: General.OptionsFileName
View.GeneralizedRaiseY
¶Generalized elevation of the view along Y-axis (in model coordinates, using formula possibly containing x, y, z, s[tep], t[ime], v0, ... v8)
Default value: "v1"
Saved in: General.OptionsFileName
View.GeneralizedRaiseZ
¶Generalized elevation of the view along Z-axis (in model coordinates, using formula possibly containing x, y, z, s[tep], t[ime], v0, ... v8)
Default value: "v2"
Saved in: General.OptionsFileName
View.Group
¶Group to which this view belongs
Default value: ""
Saved in: General.OptionsFileName
View.Name
¶Default post-processing view name
Default value: ""
Saved in: -
View.Stipple0
¶First stippling pattern
Default value: "1*0x1F1F"
Saved in: General.OptionsFileName
View.Stipple1
¶Second stippling pattern
Default value: "1*0x3333"
Saved in: General.OptionsFileName
View.Stipple2
¶Third stippling pattern
Default value: "1*0x087F"
Saved in: General.OptionsFileName
View.Stipple3
¶Fourth stippling pattern
Default value: "1*0xCCCF"
Saved in: General.OptionsFileName
View.Stipple4
¶Fifth stippling pattern
Default value: "2*0x1111"
Saved in: General.OptionsFileName
View.Stipple5
¶Sixth stippling pattern
Default value: "2*0x0F0F"
Saved in: General.OptionsFileName
View.Stipple6
¶Seventh stippling pattern
Default value: "1*0xCFFF"
Saved in: General.OptionsFileName
View.Stipple7
¶Eighth stippling pattern
Default value: "2*0x0202"
Saved in: General.OptionsFileName
View.Stipple8
¶Ninth stippling pattern
Default value: "2*0x087F"
Saved in: General.OptionsFileName
View.Stipple9
¶Tenth stippling pattern
Default value: "1*0xFFFF"
Saved in: General.OptionsFileName
View.AbscissaRangeType
¶Ascissa scale range type (1: default, 2: custom)
Default value: 1
Saved in: General.OptionsFileName
View.AdaptVisualizationGrid
¶Use adaptive visualization grid (for high-order elements)?
Default value: 0
Saved in: General.OptionsFileName
View.AngleSmoothNormals
¶Threshold angle below which normals are not smoothed
Default value: 30
Saved in: General.OptionsFileName
View.ArrowSizeMax
¶Maximum display size of arrows (in pixels)
Default value: 60
Saved in: General.OptionsFileName
View.ArrowSizeMin
¶Minimum display size of arrows (in pixels)
Default value: 0
Saved in: General.OptionsFileName
View.AutoPosition
¶Position the scale or 2D plot automatically (0: manual, 1: automatic, 2: top left, 3: top right, 4: bottom left, 5: bottom right, 6: top, 7: bottom, 8: left, 9: right, 10: full, 11: top third, 12: in model coordinates)
Default value: 1
Saved in: General.OptionsFileName
View.Axes
¶Axes (0: none, 1: simple axes, 2: box, 3: full grid, 4: open grid, 5: ruler)
Default value: 0
Saved in: General.OptionsFileName
View.AxesMikado
¶Mikado axes style
Default value: 0
Saved in: General.OptionsFileName
View.AxesAutoPosition
¶Position the axes automatically
Default value: 1
Saved in: General.OptionsFileName
View.AxesMaxX
¶Maximum X-axis coordinate
Default value: 1
Saved in: General.OptionsFileName
View.AxesMaxY
¶Maximum Y-axis coordinate
Default value: 1
Saved in: General.OptionsFileName
View.AxesMaxZ
¶Maximum Z-axis coordinate
Default value: 1
Saved in: General.OptionsFileName
View.AxesMinX
¶Minimum X-axis coordinate
Default value: 0
Saved in: General.OptionsFileName
View.AxesMinY
¶Minimum Y-axis coordinate
Default value: 0
Saved in: General.OptionsFileName
View.AxesMinZ
¶Minimum Z-axis coordinate
Default value: 0
Saved in: General.OptionsFileName
View.AxesTicsX
¶Number of tics on the X-axis
Default value: 5
Saved in: General.OptionsFileName
View.AxesTicsY
¶Number of tics on the Y-axis
Default value: 5
Saved in: General.OptionsFileName
View.AxesTicsZ
¶Number of tics on the Z-axis
Default value: 5
Saved in: General.OptionsFileName
View.Boundary
¶Draw the ‘N minus b’-dimensional boundary of the element (N: element dimension, b: option value)
Default value: 0
Saved in: General.OptionsFileName
View.CenterGlyphs
¶Center glyphs (arrows, numbers, etc.)? (0: left, 1: centered, 2: right)
Default value: 0
Saved in: General.OptionsFileName
View.Clip
¶Enable clipping planes? (Plane[i]=2^i, i=0,...,5)
Default value: 0
Saved in: -
View.Closed
¶Close the subtree containing this view
Default value: 0
Saved in: General.OptionsFileName
View.ColormapAlpha
¶Colormap alpha channel value (used only if != 1)
Default value: 1
Saved in: General.OptionsFileName
View.ColormapAlphaPower
¶Colormap alpha channel power
Default value: 0
Saved in: General.OptionsFileName
View.ColormapBeta
¶Colormap beta parameter (gamma = 1-beta)
Default value: 0
Saved in: General.OptionsFileName
View.ColormapBias
¶Colormap bias
Default value: 0
Saved in: General.OptionsFileName
View.ColormapCurvature
¶Colormap curvature or slope coefficient
Default value: 0
Saved in: General.OptionsFileName
View.ColormapInvert
¶Invert the color values, i.e., replace x with (255-x) in the colormap?
Default value: 0
Saved in: General.OptionsFileName
View.ColormapNumber
¶Default colormap number (0: black, 1: vis5d, 2: jet, 3: lucie, 4: rainbow, 5: emc2000, 6: incadescent, 7: hot, 8: pink, 9: grayscale, 10: french, 11: hsv, 12: spectrum, 13: bone, 14: spring, 15: summer, 16: autumm, 17: winter, 18: cool, 19: copper, 20: magma, 21: inferno, 22: plasma, 23: viridis, 24: turbo)
Default value: 2
Saved in: General.OptionsFileName
View.ColormapRotation
¶Incremental colormap rotation
Default value: 0
Saved in: General.OptionsFileName
View.ColormapSwap
¶Swap the min/max values in the colormap?
Default value: 0
Saved in: General.OptionsFileName
View.ComponentMap0
¶Forced component 0 (if View.ForceComponents > 0)
Default value: 0
Saved in: General.OptionsFileName
View.ComponentMap1
¶Forced component 1 (if View.ForceComponents > 0)
Default value: 1
Saved in: General.OptionsFileName
View.ComponentMap2
¶Forced component 2 (if View.ForceComponents > 0)
Default value: 2
Saved in: General.OptionsFileName
View.ComponentMap3
¶Forced component 3 (if View.ForceComponents > 0)
Default value: 3
Saved in: General.OptionsFileName
View.ComponentMap4
¶Forced component 4 (if View.ForceComponents > 0)
Default value: 4
Saved in: General.OptionsFileName
View.ComponentMap5
¶Forced component 5 (if View.ForceComponents > 0)
Default value: 5
Saved in: General.OptionsFileName
View.ComponentMap6
¶Forced component 6 (if View.ForceComponents > 0)
Default value: 6
Saved in: General.OptionsFileName
View.ComponentMap7
¶Forced component 7 (if View.ForceComponents > 0)
Default value: 7
Saved in: General.OptionsFileName
View.ComponentMap8
¶Forced component 8 (if View.ForceComponents > 0)
Default value: 8
Saved in: General.OptionsFileName
View.CustomAbscissaMax
¶User-defined maximum abscissa value
Default value: 0
Saved in: -
View.CustomAbscissaMin
¶User-defined minimum abscissa value
Default value: 0
Saved in: -
View.CustomMax
¶User-defined maximum value to be displayed
Default value: 0
Saved in: -
View.CustomMin
¶User-defined minimum value to be displayed
Default value: 0
Saved in: -
View.DisplacementFactor
¶Displacement amplification
Default value: 1
Saved in: General.OptionsFileName
View.DrawHexahedra
¶Display post-processing hexahedra?
Default value: 1
Saved in: General.OptionsFileName
View.DrawLines
¶Display post-processing lines?
Default value: 1
Saved in: General.OptionsFileName
View.DrawPoints
¶Display post-processing points?
Default value: 1
Saved in: General.OptionsFileName
View.DrawPrisms
¶Display post-processing prisms?
Default value: 1
Saved in: General.OptionsFileName
View.DrawPyramids
¶Display post-processing pyramids?
Default value: 1
Saved in: General.OptionsFileName
View.DrawTrihedra
¶Display post-processing trihedra?
Default value: 1
Saved in: General.OptionsFileName
View.DrawQuadrangles
¶Display post-processing quadrangles?
Default value: 1
Saved in: General.OptionsFileName
View.DrawScalars
¶Display scalar values?
Default value: 1
Saved in: General.OptionsFileName
View.DrawSkinOnly
¶Draw only the skin of 3D scalar views?
Default value: 0
Saved in: General.OptionsFileName
View.DrawStrings
¶Display post-processing annotation strings?
Default value: 1
Saved in: General.OptionsFileName
View.DrawTensors
¶Display tensor values?
Default value: 1
Saved in: General.OptionsFileName
View.DrawTetrahedra
¶Display post-processing tetrahedra?
Default value: 1
Saved in: General.OptionsFileName
View.DrawTriangles
¶Display post-processing triangles?
Default value: 1
Saved in: General.OptionsFileName
View.DrawVectors
¶Display vector values?
Default value: 1
Saved in: General.OptionsFileName
View.Explode
¶Element shrinking factor (between 0 and 1)
Default value: 1
Saved in: General.OptionsFileName
View.ExternalView
¶Index of the view used to color vector fields (-1: self)
Default value: -1
Saved in: General.OptionsFileName
View.FakeTransparency
¶Use fake transparency (cheaper than the real thing, but incorrect)
Default value: 0
Saved in: General.OptionsFileName
View.ForceNumComponents
¶Force number of components to display (see View.ComponentMapN for mapping)
Default value: 0
Saved in: General.OptionsFileName
View.GeneralizedRaiseFactor
¶Generalized raise amplification factor
Default value: 1
Saved in: General.OptionsFileName
View.GeneralizedRaiseView
¶Index of the view used for generalized raise (-1: self)
Default value: -1
Saved in: General.OptionsFileName
View.GlyphLocation
¶Glyph (arrow, number, etc.) location (1: center of gravity, 2: node)
Default value: 1
Saved in: General.OptionsFileName
View.Height
¶Height (in pixels) of the scale or 2D plot
Default value: 200
Saved in: General.OptionsFileName
View.IntervalsType
¶Type of interval display (1: iso, 2: continuous, 3: discrete, 4: numeric)
Default value: 2
Saved in: General.OptionsFileName
View.Light
¶Enable lighting for the view
Default value: 1
Saved in: General.OptionsFileName
View.LightLines
¶Light element edges
Default value: 1
Saved in: General.OptionsFileName
View.LightTwoSide
¶Light both sides of surfaces (leads to slower rendering)
Default value: 1
Saved in: General.OptionsFileName
View.LineType
¶Display lines as solid color segments (0) or 3D cylinders (1)
Default value: 0
Saved in: General.OptionsFileName
View.LineWidth
¶Display width of lines (in pixels)
Default value: 1
Saved in: General.OptionsFileName
View.MaxRecursionLevel
¶Maximum recursion level for adaptive views
Default value: 0
Saved in: General.OptionsFileName
View.Max
¶Maximum value in the view (read-only)
Default value: 0
Saved in: -
View.MaxVisible
¶Maximum value in the visible parts of the view, taking current time step and tensor display type into account (read-only)
Default value: 0
Saved in: -
View.MaxX
¶Maximum view coordinate along the X-axis (read-only)
Default value: 0
Saved in: -
View.MaxY
¶Maximum view coordinate along the Y-axis (read-only)
Default value: 0
Saved in: -
View.MaxZ
¶Maximum view coordinate along the Z-axis (read-only)
Default value: 0
Saved in: -
View.Min
¶Minimum value in the view (read-only)
Default value: 0
Saved in: -
View.MinVisible
¶Minimum value in the visible parts of the view, taking current time step and tensor display type into account (read-only)
Default value: 0
Saved in: -
View.MinX
¶Minimum view coordinate along the X-axis (read-only)
Default value: 0
Saved in: -
View.MinY
¶Minimum view coordinate along the Y-axis (read-only)
Default value: 0
Saved in: -
View.MinZ
¶Minimum view coordinate along the Z-axis (read-only)
Default value: 0
Saved in: -
View.NbIso
¶Number of intervals
Default value: 10
Saved in: General.OptionsFileName
View.NbTimeStep
¶Number of time steps in the view (do not change this!)
Default value: 1
Saved in: -
View.NormalRaise
¶Elevation of the view along the normal (in model coordinates)
Default value: 0
Saved in: -
View.Normals
¶Display size of normal vectors (in pixels)
Default value: 0
Saved in: General.OptionsFileName
View.OffsetX
¶Translation of the view along X-axis (in model coordinates)
Default value: 0
Saved in: -
View.OffsetY
¶Translation of the view along Y-axis (in model coordinates)
Default value: 0
Saved in: -
View.OffsetZ
¶Translation of the view along Z-axis (in model coordinates)
Default value: 0
Saved in: -
View.PointSize
¶Display size of points (in pixels)
Default value: 3
Saved in: General.OptionsFileName
View.PointType
¶Display points as solid color dots (0), 3D spheres (1), scaled dots (2) or scaled spheres (3)
Default value: 0
Saved in: General.OptionsFileName
View.PositionX
¶X position (in pixels) of the scale or 2D plot (< 0: measure from right edge; >= 1e5: centered)
Default value: 100
Saved in: General.OptionsFileName
View.PositionY
¶Y position (in pixels) of the scale or 2D plot (< 0: measure from bottom edge; >= 1e5: centered)
Default value: 50
Saved in: General.OptionsFileName
View.RaiseX
¶Elevation of the view along X-axis (in model coordinates)
Default value: 0
Saved in: -
View.RaiseY
¶Elevation of the view along Y-axis (in model coordinates)
Default value: 0
Saved in: -
View.RaiseZ
¶Elevation of the view along Z-axis (in model coordinates)
Default value: 0
Saved in: -
View.RangeType
¶Value scale range type (1: default, 2: custom, 3: per time step)
Default value: 1
Saved in: General.OptionsFileName
View.Sampling
¶Element sampling rate (draw one out every ‘Sampling’ elements)
Default value: 1
Saved in: General.OptionsFileName
View.SaturateValues
¶Saturate the view values to custom min and max (1: true, 0: false)
Default value: 0
Saved in: General.OptionsFileName
View.ScaleType
¶Value scale type (1: linear, 2: logarithmic, 3: double logarithmic)
Default value: 1
Saved in: General.OptionsFileName
View.ShowElement
¶Show element boundaries?
Default value: 0
Saved in: General.OptionsFileName
View.ShowScale
¶Show value scale?
Default value: 1
Saved in: General.OptionsFileName
View.ShowTime
¶Time display mode (0: none, 1: time series, 2: harmonic data, 3: automatic, 4: step data, 5: multi-step data, 6: real eigenvalues, 7: complex eigenvalues)
Default value: 3
Saved in: General.OptionsFileName
View.SmoothNormals
¶Smooth the normals?
Default value: 0
Saved in: General.OptionsFileName
View.Stipple
¶Stipple curves in 2D and line plots?
Default value: 0
Saved in: General.OptionsFileName
View.Tangents
¶Display size of tangent vectors (in pixels)
Default value: 0
Saved in: General.OptionsFileName
View.TargetError
¶Target representation error for adaptive views
Default value: 0.01
Saved in: General.OptionsFileName
View.TensorType
¶Tensor display type (1: Von-Mises, 2: maximum eigenvalue, 3: minimum eigenvalue, 4: eigenvectors, 5: ellipse, 6: ellipsoid, 7: frame)
Default value: 1
Saved in: General.OptionsFileName
View.TimeStep
¶Current time step displayed
Default value: 0
Saved in: -
View.Time
¶Current time displayed (if positive, sets the time step corresponding the given time value)
Default value: 0
Saved in: -
View.TransformXX
¶Element (1,1) of the 3x3 coordinate transformation matrix
Default value: 1
Saved in: -
View.TransformXY
¶Element (1,2) of the 3x3 coordinate transformation matrix
Default value: 0
Saved in: -
View.TransformXZ
¶Element (1,3) of the 3x3 coordinate transformation matrix
Default value: 0
Saved in: -
View.TransformYX
¶Element (2,1) of the 3x3 coordinate transformation matrix
Default value: 0
Saved in: -
View.TransformYY
¶Element (2,2) of the 3x3 coordinate transformation matrix
Default value: 1
Saved in: -
View.TransformYZ
¶Element (2,3) of the 3x3 coordinate transformation matrix
Default value: 0
Saved in: -
View.TransformZX
¶Element (3,1) of the 3x3 coordinate transformation matrix
Default value: 0
Saved in: -
View.TransformZY
¶Element (3,2) of the 3x3 coordinate transformation matrix
Default value: 0
Saved in: -
View.TransformZZ
¶Element (3,3) of the 3x3 coordinate transformation matrix
Default value: 1
Saved in: -
View.Type
¶Type of plot (1: 3D, 2: 2D space, 3: 2D time, 4: 2D)
Default value: 1
Saved in: -
View.UseGeneralizedRaise
¶Use generalized raise?
Default value: 0
Saved in: General.OptionsFileName
View.VectorType
¶Vector display type (1: segment, 2: arrow, 3: pyramid, 4: 3D arrow, 5: displacement, 6: comet)
Default value: 4
Saved in: General.OptionsFileName
View.Visible
¶Is the view visible?
Default value: 1
Saved in: -
View.Width
¶Width (in pixels) of the scale or 2D plot
Default value: 300
Saved in: General.OptionsFileName
View.Color.Points
¶Point color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Lines
¶Line color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Triangles
¶Triangle color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Quadrangles
¶Quadrangle color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Tetrahedra
¶Tetrahedron color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Hexahedra
¶Hexahedron color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Prisms
¶Prism color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Pyramids
¶Pyramid color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Trihedra
¶Trihedron color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Tangents
¶Tangent vector color
Default value: {255,255,0}
Saved in: General.OptionsFileName
View.Color.Normals
¶Normal vector color
Default value: {255,0,0}
Saved in: General.OptionsFileName
View.Color.Text2D
¶2D text color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Text3D
¶3D text color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Axes
¶Axes color
Default value: {0,0,0}
Saved in: General.OptionsFileName
View.Color.Background2D
¶Bacground color for 2D plots
Default value: {255,255,255}
Saved in: General.OptionsFileName
View.ColorTable
¶Color table used to draw the view
Saved in: General.OptionsFileName
Stable releases and source snapshots are available from https://gmsh.info/src/. You can also access the Git repository directly:
git clone https://gitlab.onelab.info/gmsh/gmsh.git
git pull
Once you have the source code, you need to run CMake to configure your build (see the README.txt file in the top-level source directory for detailed information on how to run CMake).
Each build can be configured using a series of options, to selectively enable optional modules or features. Here is the list of CMake options:
ENABLE_3M
Enable proprietary 3M extension (default: OFF)
ENABLE_ALGLIB
Enable ALGLIB (used by some mesh optimizers) (default: ON)
ENABLE_ANN
Enable ANN (used for fast point search in mesh/post) (default: ON)
ENABLE_BAMG
Enable Bamg 2D anisotropic mesh generator (default: ON)
ENABLE_BLAS_LAPACK
Enable BLAS/Lapack for linear algebra (if Eigen if disabled) (default: OFF)
ENABLE_BLOSSOM
Enable Blossom algorithm (needed for full quad meshing) (default: ON)
ENABLE_BUILD_LIB
Enable ’lib’ target for building static Gmsh library (default: OFF)
ENABLE_BUILD_SHARED
Enable ’shared’ target for building shared Gmsh library (default: OFF)
ENABLE_BUILD_DYNAMIC
Enable dynamic Gmsh executable (linked with shared library) (default: OFF)
ENABLE_BUILD_ANDROID
Enable Android NDK library target (experimental) (default: OFF)
ENABLE_BUILD_IOS
Enable iOS library target (experimental) (default: OFF)
ENABLE_CGNS
Enable CGNS import/export (experimental) (default: ON)
ENABLE_CGNS_CPEX0045
Enable high-order CGNS import/export following CPEX0045 (experimental) (default: OFF)
ENABLE_CAIRO
Enable Cairo to render fonts (experimental) (default: ON)
ENABLE_PROFILE
Enable profiling compiler flags (default: OFF)
ENABLE_DINTEGRATION
Enable discrete integration (needed for levelsets) (default: ON)
ENABLE_DOMHEX
Enable experimental DOMHEX code (default: ON)
ENABLE_EIGEN
Enable Eigen for linear algebra (instead of Blas/Lapack) (default: ON)
ENABLE_FLTK
Enable FLTK graphical user interface (requires mesh/post) (default: ON)
ENABLE_GETDP
Enable GetDP solver (linked as a library, experimental) (default: ON)
ENABLE_GMM
Enable GMM linear solvers (simple alternative to PETSc) (default: ON)
ENABLE_GMP
Enable GMP for Kbipack (advanced) (default: ON)
ENABLE_GRAPHICS
Enable building graphics lib even without GUI (advanced) (default: OFF)
ENABLE_HXT
Enable HXT library (for reparametrization and meshing) (default: ON)
ENABLE_KBIPACK
Enable Kbipack (neeeded by homology solver) (default: ON)
ENABLE_MATHEX
Enable Mathex expression parser (used by plugins and options) (default: ON)
ENABLE_MED
Enable MED mesh and post file formats (default: ON)
ENABLE_MESH
Enable mesh module (required by GUI) (default: ON)
ENABLE_METIS
Enable Metis mesh partitioner (default: ON)
ENABLE_MMG
Enable Mmg mesh adaptation interface (default: ON)
ENABLE_MPEG_ENCODE
Enable built-in MPEG movie encoder (default: ON)
ENABLE_MPI
Enable MPI (experimental, not used for meshing) (default: OFF)
ENABLE_MSVC_STATIC_RUNTIME
Enable static Visual C++ runtime (default: OFF)
ENABLE_MUMPS
Enable MUMPS sparse direct linear solver (default: OFF)
ENABLE_NETGEN
Enable Netgen 3D frontal mesh generator (default: ON)
ENABLE_NUMPY
Enable fullMatrix and numpy array conversion for private API (default: OFF)
ENABLE_PETSC4PY
Enable petsc4py wrappers for petsc matrices for private API (default: OFF)
ENABLE_OCC
Enable OpenCASCADE CAD kernel (default: ON)
ENABLE_OCC_CAF
Enable OpenCASCADE CAF module (for STEP/IGES attributes) (default: ON)
ENABLE_OCC_STATIC
Link OpenCASCADE static instead of dynamic libraries (requires ENABLE_OCC) (default: OFF)
ENABLE_OCC_TBB
Add TBB libraries in list of OCC libraries (default: OFF)
ENABLE_ONELAB
Enable ONELAB solver interface (default: ON)
ENABLE_ONELAB_METAMODEL
Enable ONELAB metamodels (experimental) (default: ON)
ENABLE_OPENACC
Enable OpenACC (default: OFF)
ENABLE_OPENMP
Enable OpenMP (default: OFF)
ENABLE_OPTHOM
Enable high-order mesh optimization tools (default: ON)
ENABLE_OS_SPECIFIC_INSTALL
Enable OS-specific (e.g. app bundle) installation (default: OFF)
ENABLE_OSMESA
Enable OSMesa for offscreen rendering (experimental) (default: OFF)
ENABLE_P4EST
Enable p4est for enabling automatic mesh size field (experimental) (default: OFF)
ENABLE_PACKAGE_STRIP
Strip symbols in install packages to reduce install size (default: ON)
ENABLE_PARSER
Enable GEO file parser (required for .geo/.pos scripts) (default: ON)
ENABLE_PETSC
Enable PETSc linear solvers (required for SLEPc) (default: OFF)
ENABLE_PLUGINS
Enable post-processing plugins (default: ON)
ENABLE_POST
Enable post-processing module (required by GUI) (default: ON)
ENABLE_POPPLER
Enable Poppler for displaying PDF documents (experimental) (default: OFF)
ENABLE_PRIVATE_API
Enable private API (default: OFF)
ENABLE_PRO
Enable PRO extensions (default: ON)
ENABLE_QUADTRI
Enable QuadTri structured meshing extensions (default: ON)
ENABLE_REVOROPT
Enable Revoropt (used for CVT remeshing) (default: OFF)
ENABLE_RPATH
Use RPATH in dynamically linked targets (default: ON)
ENABLE_SLEPC
Enable SLEPc eigensolvers (default: OFF)
ENABLE_SOLVER
Enable built-in finite element solvers (required for reparametrization) (default: ON)
ENABLE_SYSTEM_CONTRIB
Use system versions of contrib libraries, when possible (default: OFF)
ENABLE_TCMALLOC
Enable libtcmalloc (fast malloc that does not release memory) (default: OFF)
ENABLE_TESTS
Enable tests (default: ON)
ENABLE_TOUCHBAR
Enable Apple Touch bar (default: ON)
ENABLE_VISUDEV
Enable additional visualization capabilities for development purposes (default: OFF)
ENABLE_VOROPP
Enable voro++ (for hex meshing, experimental) (default: ON)
ENABLE_WRAP_JAVA
Generate SWIG Java wrappers for private API (default: OFF)
ENABLE_WRAP_PYTHON
Generate SWIG Python wrappers for private API (not used by public API) (default: OFF)
ENABLE_ZIPPER
Enable Zip file compression/decompression (default: OFF)
The wiki (https://gitlab.onelab.info/gmsh/gmsh/wikis/Gmsh-compilation) contains more detailed instructions on how to compile Gmsh, including the compilation of common dependencies.
Next: Information for developers, Previous: Compiling the source code, Up: Gmsh [Contents][Index]
The Gmsh Application Programming Interface (API) allows you to integrate the Gmsh library in your own application. By design, the Gmsh API is purely functional, and only uses elementary types from the target language. Currently supported languages are C++, C, Python and Julia. See the tutorial/c++, tutorial/c, tutorial/python and tutorial/julia directories from the Tutorial for examples. For other API examples, see the demos/api directory.
The different versions of the API are generated automatically from the master API definition file api/gen.py:
The additional
gmsh.h_cwrap
header redefines the C++ API in terms of the C API. This is provided as
a convenience for users of the binary Gmsh
Software Development Kit (SDK) whose C++ compiler Application Binary
Interface (ABI) is not compatible with the ABI of the C++ compiler used
to create the SDK. To use these C++ bindings of the C API instead of the
native C++ API, simply rename gmsh.h_cwrap
as gmsh.h
. Note
that this will lead to (slightly) reduced performance compared to using
the native Gmsh C++ API, as it entails additional data copies between
the C++ wrapper, the C API and the native C++ code.
The structure of the API reflects the underlying Gmsh data model (see also Source code structure):
gmsh/model
and gmsh/view
,
respectively. The other top-level namespaces are gmsh/option
(which handles all options), gmsh/plugin
(which handles
extensions to core Gmsh functionality), gmsh/graphics
(which
handles drawing), gmsh/fltk
(which handles the graphical user
interface), gmsh/onelab
(which handles ONELAB parameters and
communications with external codes) and gmsh/logger
(which
handles information logging).
gmsh/model/geo
or gmsh/model/occ
namespaces,
respectively), as Gmsh does not translate across CAD formats but rather
directly accesses the native representation. CAD entities must be
synchronized with the model in order to be meshed, or, more
generally, for functions outside of gmsh/model/geo
or
gmsh/model/occ
to manipulate them. 1D and 2D meshing algorithms
use the parametrization of the underlying geometrical curve or
surface to generate the mesh. Discrete entities can be remeshed provided
that a parametrization is explicitly recomputed for them.
gmsh/model/mesh
namespace.
All the functions available in the API are given below. See the relevant
header/module file for the exact definition in each supported language:
in C++
gmsh/model/geo/addPoint
will lead to a namespaced function
gmsh::model::geo::addPoint
, while in
Python and
Julia it will lead to
gmsh.model.geo.addPoint
, and in
C to
gmshModelGeoAddPoint
. In addition to the default “camelCase”
function names, the Python and Julia APIs also define “snake case”
aliases, i.e. gmsh.model.geo.add_point
, as this is the
recommended style in these languages. Output values are passed by
reference in C++, as pointers in C and directly returned (after the
return value, if any) in Python and Julia.
gmsh
: top-level functionsgmsh/option
: option handling functionsgmsh/model
: model functionsgmsh/model/mesh
: mesh functionsgmsh/model/mesh/field
: mesh size field functionsgmsh/model/geo
: built-in CAD kernel functionsgmsh/model/geo/mesh
: built-in CAD kernel meshing constraintsgmsh/model/occ
: OpenCASCADE CAD kernel functionsgmsh/model/occ/mesh
: OpenCASCADE CAD kernel meshing constraintsgmsh/view
: post-processing view functionsgmsh/plugin
: plugin functionsgmsh/graphics
: graphics functionsgmsh/fltk
: FLTK graphical user interface functionsgmsh/onelab
: ONELAB server functionsgmsh/logger
: information logging functionsgmsh
: top-level functionsgmsh/initialize
¶Initialize Gmsh API. This must be called before any call to the other functions
in the API. If argc
and argv
(or just argv
in Python or
Julia) are provided, they will be handled in the same way as the command line
arguments in the Gmsh app. If readConfigFiles
is set, read system Gmsh
configuration files (gmshrc and gmsh-options). Initializing the API sets the
options "General.Terminal" to 1 and "General.AbortOnError" to 2.
gmsh/finalize
¶Finalize the Gmsh API. This must be called when you are done using the Gmsh API.
gmsh/open
¶Open a file. Equivalent to the File->Open
menu in the Gmsh app. Handling
of the file depends on its extension and/or its contents: opening a file with
model data will create a new model.
fileName
-
-
C++ (x1.cpp, explore.cpp, onelab_data.cpp, open.cpp), Python (x1.py, explore.py, flatten.py, heal.py, onelab_data.py, ...)
gmsh/merge
¶Merge a file. Equivalent to the File->Merge
menu in the Gmsh app.
Handling of the file depends on its extension and/or its contents. Merging a
file with model data will add the data to the current model.
gmsh/write
¶Write a file. The export format is determined by the file extension.
gmsh/clear
¶Clear all loaded models and post-processing data, and add a new empty model.
Next: Namespace gmsh/model
: model functions, Previous: Namespace gmsh
: top-level functions, Up: Gmsh API [Contents][Index]
gmsh/option
: option handling functionsgmsh/option/setNumber
¶Set a numerical option to value
. name
is of the form
"category.option" or "category[num].option". Available categories and options
are listed in the Gmsh reference manual.
gmsh/option/getNumber
¶Get the value
of a numerical option. name
is of the form
"category.option" or "category[num].option". Available categories and options
are listed in the Gmsh reference manual.
gmsh/option/setString
¶Set a string option to value
. name
is of the form
"category.option" or "category[num].option". Available categories and options
are listed in the Gmsh reference manual.
gmsh/option/getString
¶Get the value
of a string option. name
is of the form
"category.option" or "category[num].option". Available categories and options
are listed in the Gmsh reference manual.
gmsh/option/setColor
¶Set a color option to the RGBA value (r
, g
, b
, a
),
where where r
, g
, b
and a
should be integers between
0 and 255. name
is of the form "category.option" or
"category[num].option". Available categories and options are listed in the Gmsh
reference manual, with the "Color." middle string removed.
gmsh/option/getColor
¶Get the r
, g
, b
, a
value of a color option.
name
is of the form "category.option" or "category[num].option".
Available categories and options are listed in the Gmsh reference manual, with
the "Color." middle string removed.
Next: Namespace gmsh/model/mesh
: mesh functions, Previous: Namespace gmsh/option
: option handling functions, Up: Gmsh API [Contents][Index]
gmsh/model
: model functionsgmsh/model/add
¶Add a new model, with name name
, and set it as the current model.
gmsh/model/remove
¶Remove the current model.
gmsh/model/list
¶List the names of all models.
gmsh/model/getCurrent
¶Get the name of the current model.
gmsh/model/setCurrent
¶Set the current model to the model with name name
. If several models have
the same name, select the one that was added first.
name
-
-
Python (copy_mesh.py)
gmsh/model/getFileName
¶Get the file name (if any) associated with the current model. A file name is associated when a model is read from a file on disk.
gmsh/model/setFileName
¶Set the file name associated with the current model.
gmsh/model/getEntities
¶Get all the entities in the current model. If dim
is >= 0, return only
the entities of the specified dimension (e.g. points if dim
== 0). The
entities are returned as a vector of (dim, tag) integer pairs.
gmsh/model/setEntityName
¶Set the name of the entity of dimension dim
and tag tag
.
gmsh/model/getEntityName
¶Get the name of the entity of dimension dim
and tag tag
.
gmsh/model/getPhysicalGroups
¶Get all the physical groups in the current model. If dim
is >= 0, return
only the entities of the specified dimension (e.g. physical points if dim
== 0). The entities are returned as a vector of (dim, tag) integer pairs.
dim = -1
dimTags
-
Python (poisson.py)
gmsh/model/getEntitiesForPhysicalGroup
¶Get the tags of the model entities making up the physical group of dimension
dim
and tag tag
.
gmsh/model/getPhysicalGroupsForEntity
¶Get the tags of the physical groups (if any) to which the model entity of
dimension dim
and tag tag
belongs.
gmsh/model/addPhysicalGroup
¶Add a physical group of dimension dim
, grouping the model entities with
tags tags
. Return the tag of the physical group, equal to tag
if
tag
is positive, or a new tag if tag
< 0.
gmsh/model/removePhysicalGroups
¶Remove the physical groups dimTags
from the current model. If
dimTags
is empty, remove all groups.
gmsh/model/setPhysicalName
¶Set the name of the physical group of dimension dim
and tag tag
.
gmsh/model/removePhysicalName
¶Remove the physical name name
from the current model.
gmsh/model/getPhysicalName
¶Get the name of the physical group of dimension dim
and tag tag
.
gmsh/model/getBoundary
¶Get the boundary of the model entities dimTags
. Return in
outDimTags
the boundary of the individual entities (if combined
is
false) or the boundary of the combined geometrical shape formed by all input
entities (if combined
is true). Return tags multiplied by the sign of the
boundary entity if oriented
is true. Apply the boundary operator
recursively down to dimension 0 (i.e. to points) if recursive
is true.
gmsh/model/getAdjacencies
¶Get the upward and downward adjacencies of the model entity of dimension
dim
and tag tag
. The upward
vector returns the adjacent
entities of dimension dim
+ 1; the downward
vector returns the
adjacent entities of dimension dim
- 1.
gmsh/model/getEntitiesInBoundingBox
¶Get the model entities in the bounding box defined by the two points
(xmin
, ymin
, zmin
) and (xmax
, ymax
,
zmax
). If dim
is >= 0, return only the entities of the specified
dimension (e.g. points if dim
== 0).
gmsh/model/getBoundingBox
¶Get the bounding box (xmin
, ymin
, zmin
), (xmax
,
ymax
, zmax
) of the model entity of dimension dim
and tag
tag
. If dim
and tag
are negative, get the bounding box of
the whole model.
gmsh/model/getDimension
¶Get the geometrical dimension of the current model.
gmsh/model/addDiscreteEntity
¶Add a discrete model entity (defined by a mesh) of dimension dim
in the
current model. Return the tag of the new discrete entity, equal to tag
if
tag
is positive, or a new tag if tag
< 0. boundary
specifies the tags of the entities on the boundary of the discrete entity, if
any. Specifying boundary
allows Gmsh to construct the topology of the
overall model.
dim
, tag = -1
, boundary = []
-
integer value
C++ (x2.cpp, x4.cpp, discrete.cpp, edges.cpp, faces.cpp, ...), Python (x2.py, x4.py, copy_mesh.py, discrete.py, import_perf.py, ...)
gmsh/model/removeEntities
¶Remove the entities dimTags
of the current model. If recursive
is
true, remove all the entities on their boundaries, down to dimension 0.
gmsh/model/removeEntityName
¶Remove the entity name name
from the current model.
gmsh/model/getType
¶Get the type of the entity of dimension dim
and tag tag
.
dim
, tag
entityType
-
C++ (t21.cpp, x1.cpp, explore.cpp, partition.cpp), Python (t21.py, x1.py, explore.py, partition.py)
gmsh/model/getParent
¶In a partitioned model, get the parent of the entity of dimension dim
and
tag tag
, i.e. from which the entity is a part of, if any.
parentDim
and parentTag
are set to -1 if the entity has no parent.
dim
, tag
parentDim
, parentTag
-
C++ (t21.cpp, x1.cpp, explore.cpp, partition.cpp), Python (t21.py, x1.py, explore.py, partition.py)
gmsh/model/getPartitions
¶In a partitioned model, return the tags of the partition(s) to which the entity belongs.
dim
, tag
partitions
-
C++ (t21.cpp, x1.cpp, explore.cpp, partition.cpp), Python (t21.py, x1.py, explore.py, partition.py)
gmsh/model/getValue
¶Evaluate the parametrization of the entity of dimension dim
and tag
tag
at the parametric coordinates parametricCoord
. Only valid for
dim
equal to 0 (with empty parametricCoord
), 1 (with
parametricCoord
containing parametric coordinates on the curve) or 2
(with parametricCoord
containing pairs of u, v parametric coordinates on
the surface, concatenated: [p1u, p1v, p2u, ...]). Return triplets of x, y, z
coordinates in coord
, concatenated: [p1x, p1y, p1z, p2x, ...].
dim
, tag
, parametricCoord
coord
-
C++ (t2.cpp), Python (t2.py, reparamOnFace.py, terrain_stl.py)
gmsh/model/getDerivative
¶Evaluate the derivative of the parametrization of the entity of dimension
dim
and tag tag
at the parametric coordinates
parametricCoord
. Only valid for dim
equal to 1 (with
parametricCoord
containing parametric coordinates on the curve) or 2
(with parametricCoord
containing pairs of u, v parametric coordinates on
the surface, concatenated: [p1u, p1v, p2u, ...]). For dim
equal to 1
return the x, y, z components of the derivative with respect to u [d1ux, d1uy,
d1uz, d2ux, ...]; for dim
equal to 2 return the x, y, z components of the
derivative with respect to u and v: [d1ux, d1uy, d1uz, d1vx, d1vy, d1vz, d2ux,
...].
gmsh/model/getSecondDerivative
¶Evaluate the second derivative of the parametrization of the entity of dimension
dim
and tag tag
at the parametric coordinates
parametricCoord
. Only valid for dim
equal to 1 (with
parametricCoord
containing parametric coordinates on the curve) or 2
(with parametricCoord
containing pairs of u, v parametric coordinates on
the surface, concatenated: [p1u, p1v, p2u, ...]). For dim
equal to 1
return the x, y, z components of the second derivative with respect to u [d1uux,
d1uuy, d1uuz, d2uux, ...]; for dim
equal to 2 return the x, y, z
components of the second derivative with respect to u and v, and the mixed
derivative with respect to u and v: [d1uux, d1uuy, d1uuz, d1vvx, d1vvy, d1vvz,
d1uvx, d1uvy, d1uvz, d2uux, ...].
gmsh/model/getCurvature
¶Evaluate the (maximum) curvature of the entity of dimension dim
and tag
tag
at the parametric coordinates parametricCoord
. Only valid for
dim
equal to 1 (with parametricCoord
containing parametric
coordinates on the curve) or 2 (with parametricCoord
containing pairs of
u, v parametric coordinates on the surface, concatenated: [p1u, p1v, p2u, ...]).
dim
, tag
, parametricCoord
curvatures
-
Python (normals.py)
gmsh/model/getPrincipalCurvatures
¶Evaluate the principal curvatures of the surface with tag tag
at the
parametric coordinates parametricCoord
, as well as their respective
directions. parametricCoord
are given by pair of u and v coordinates,
concatenated: [p1u, p1v, p2u, ...].
gmsh/model/getNormal
¶Get the normal to the surface with tag tag
at the parametric coordinates
parametricCoord
. parametricCoord
are given by pairs of u and v
coordinates, concatenated: [p1u, p1v, p2u, ...]. normals
are returned as
triplets of x, y, z components, concatenated: [n1x, n1y, n1z, n2x, ...].
tag
, parametricCoord
normals
-
Python (normals.py)
gmsh/model/getParametrization
¶Get the parametric coordinates parametricCoord
for the points
coord
on the entity of dimension dim
and tag tag
.
coord
are given as triplets of x, y, z coordinates, concatenated: [p1x,
p1y, p1z, p2x, ...]. parametricCoord
returns the parametric coordinates t
on the curve (if dim
= 1) or pairs of u and v coordinates concatenated on
the surface (if dim
= 2), i.e. [p1t, p2t, ...] or [p1u, p1v, p2u, ...].
gmsh/model/getParametrizationBounds
¶Get the min
and max
bounds of the parametric coordinates for the
entity of dimension dim
and tag tag
.
dim
, tag
min
, max
-
Python (reparamOnFace.py)
gmsh/model/isInside
¶Check if the parametric coordinates provided in parametricCoord
correspond to points inside the entitiy of dimension dim
and tag
tag
, and return the number of points inside. This feature is only
available for a subset of curves and surfaces, depending on the underyling
geometrical representation.
gmsh/model/getClosestPoint
¶Get the points closestCoord
on the entity of dimension dim
and tag
tag
to the points coord
, by orthogonal projection. coord
and closestCoord
are given as triplets of x, y, z coordinates,
concatenated: [p1x, p1y, p1z, p2x, ...]. parametricCoord
returns the
parametric coordinates t on the curve (if dim
= 1) or pairs of u and v
coordinates concatenated on the surface (if dim
= 2), i.e. [p1t, p2t,
...] or [p1u, p1v, p2u, ...].
dim
, tag
, coord
closestCoord
, parametricCoord
-
Python (closest_point.py)
gmsh/model/reparametrizeOnSurface
¶Reparametrize the boundary entity (point or curve, i.e. with dim
== 0 or
dim
== 1) of tag tag
on the surface surfaceTag
. If
dim
== 1, reparametrize all the points corresponding to the parametric
coordinates parametricCoord
. Multiple matches in case of periodic
surfaces can be selected with which
. This feature is only available for a
subset of entities, depending on the underyling geometrical representation.
dim
, tag
, parametricCoord
, surfaceTag
, which = 0
surfaceParametricCoord
-
Python (reparamOnFace.py)
gmsh/model/setVisibility
¶Set the visibility of the model entities dimTags
to value
. Apply
the visibility setting recursively if recursive
is true.
gmsh/model/getVisibility
¶Get the visibility of the model entity of dimension dim
and tag
tag
.
gmsh/model/setVisibilityPerWindow
¶Set the global visibility of the model per window to value
, where
windowIndex
identifies the window in the window list.
gmsh/model/setColor
¶Set the color of the model entities dimTags
to the RGBA value (r
,
g
, b
, a
), where r
, g
, b
and a
should be integers between 0 and 255. Apply the color setting recursively if
recursive
is true.
gmsh/model/getColor
¶Get the color of the model entity of dimension dim
and tag tag
.
dim
, tag
r
, g
, b
, a
-
Python (step_boundary_colors.py)
gmsh/model/setCoordinates
¶Set the x
, y
, z
coordinates of a geometrical point.
Next: Namespace gmsh/model/mesh/field
: mesh size field functions, Previous: Namespace gmsh/model
: model functions, Up: Gmsh API [Contents][Index]
gmsh/model/mesh
: mesh functionsgmsh/model/mesh/generate
¶Generate a mesh of the current model, up to dimension dim
(0, 1, 2 or 3).
gmsh/model/mesh/partition
¶Partition the mesh of the current model into numPart
partitions.
numPart
-
-
C++ (t21.cpp, partition.cpp), Python (t21.py, partition.py)
gmsh/model/mesh/unpartition
¶Unpartition the mesh of the current model.
gmsh/model/mesh/optimize
¶Optimize the mesh of the current model using method
(empty for default
tetrahedral mesh optimizer, "Netgen" for Netgen optimizer, "HighOrder" for
direct high-order mesh optimizer, "HighOrderElastic" for high-order elastic
smoother, "HighOrderFastCurving" for fast curving algorithm, "Laplace2D" for
Laplace smoothing, "Relocate2D" and "Relocate3D" for node relocation). If
force
is set apply the optimization also to discrete entities. If
dimTags
is given, only apply the optimizer to the given entities.
gmsh/model/mesh/recombine
¶Recombine the mesh of the current model.
gmsh/model/mesh/refine
¶Refine the mesh of the current model by uniformly splitting the elements.
gmsh/model/mesh/setOrder
¶Set the order of the elements in the mesh of the current model to order
.
order
-
-
Python (periodic.py)
gmsh/model/mesh/getLastEntityError
¶Get the last entities (if any) where a meshing error occurred. Currently only populated by the new 3D meshing algorithms.
gmsh/model/mesh/getLastNodeError
¶Get the last nodes (if any) where a meshing error occurred. Currently only populated by the new 3D meshing algorithms.
gmsh/model/mesh/clear
¶Clear the mesh, i.e. delete all the nodes and elements, for the entities
dimTags
. if dimTags
is empty, clear the whole mesh. Note that the
mesh of an entity can only be cleared if this entity is not on the boundary of
another entity with a non-empty mesh.
dimTags = []
-
-
Python (copy_mesh.py, flatten.py)
gmsh/model/mesh/getNodes
¶Get the nodes classified on the entity of dimension dim
and tag
tag
. If tag
< 0, get the nodes for all entities of dimension
dim
. If dim
and tag
are negative, get all the nodes in the
mesh. nodeTags
contains the node tags (their unique, strictly positive
identification numbers). coord
is a vector of length 3 times the length
of nodeTags
that contains the x, y, z coordinates of the nodes,
concatenated: [n1x, n1y, n1z, n2x, ...]. If dim
>= 0 and
returnParamtricCoord
is set, parametricCoord
contains the
parametric coordinates ([u1, u2, ...] or [u1, v1, u2, ...]) of the nodes, if
available. The length of parametricCoord
can be 0 or dim
times the
length of nodeTags
. If includeBoundary
is set, also return the
nodes classified on the boundary of the entity (which will be reparametrized on
the entity if dim
>= 0 in order to compute their parametric coordinates).
dim = -1
, tag = -1
, includeBoundary = False
, returnParametricCoord = True
nodeTags
, coord
, parametricCoord
-
C++ (x1.cpp, x4.cpp, adapt_mesh.cpp, explore.cpp), Python (x1.py, x4.py, adapt_mesh.py, copy_mesh.py, explore.py, ...)
gmsh/model/mesh/getNodesByElementType
¶Get the nodes classified on the entity of tag tag
, for all the elements
of type elementType
. The other arguments are treated as in
getNodes
.
gmsh/model/mesh/getNode
¶Get the coordinates and the parametric coordinates (if any) of the node with tag
tag
. This function relies on an internal cache (a vector in case of dense
node numbering, a map otherwise); for large meshes accessing nodes in bulk is
often preferable.
gmsh/model/mesh/setNode
¶Set the coordinates and the parametric coordinates (if any) of the node with tag
tag
. This function relies on an internal cache (a vector in case of dense
node numbering, a map otherwise); for large meshes accessing nodes in bulk is
often preferable.
gmsh/model/mesh/rebuildNodeCache
¶Rebuild the node cache.
gmsh/model/mesh/rebuildElementCache
¶Rebuild the element cache.
gmsh/model/mesh/getNodesForPhysicalGroup
¶Get the nodes from all the elements belonging to the physical group of dimension
dim
and tag tag
. nodeTags
contains the node tags;
coord
is a vector of length 3 times the length of nodeTags
that
contains the x, y, z coordinates of the nodes, concatenated: [n1x, n1y, n1z,
n2x, ...].
gmsh/model/mesh/addNodes
¶Add nodes classified on the model entity of dimension dim
and tag
tag
. nodeTags
contains the node tags (their unique, strictly
positive identification numbers). coord
is a vector of length 3 times the
length of nodeTags
that contains the x, y, z coordinates of the nodes,
concatenated: [n1x, n1y, n1z, n2x, ...]. The optional parametricCoord
vector contains the parametric coordinates of the nodes, if any. The length of
parametricCoord
can be 0 or dim
times the length of
nodeTags
. If the nodeTags
vector is empty, new tags are
automatically assigned to the nodes.
dim
, tag
, nodeTags
, coord
, parametricCoord = []
-
-
C++ (x2.cpp, x4.cpp, discrete.cpp, import_perf.cpp, plugin.cpp, ...), Python (x2.py, x4.py, copy_mesh.py, discrete.py, flatten.py, ...)
gmsh/model/mesh/reclassifyNodes
¶Reclassify all nodes on their associated model entity, based on the elements. Can be used when importing nodes in bulk (e.g. by associating them all to a single volume), to reclassify them correctly on model surfaces, curves, etc. after the elements have been set.
gmsh/model/mesh/relocateNodes
¶Relocate the nodes classified on the entity of dimension dim
and tag
tag
using their parametric coordinates. If tag
< 0, relocate the
nodes for all entities of dimension dim
. If dim
and tag
are
negative, relocate all the nodes in the mesh.
gmsh/model/mesh/getElements
¶Get the elements classified on the entity of dimension dim
and tag
tag
. If tag
< 0, get the elements for all entities of dimension
dim
. If dim
and tag
are negative, get all the elements in
the mesh. elementTypes
contains the MSH types of the elements (e.g.
2
for 3-node triangles: see getElementProperties
to obtain the
properties for a given element type). elementTags
is a vector of the same
length as elementTypes
; each entry is a vector containing the tags
(unique, strictly positive identifiers) of the elements of the corresponding
type. nodeTags
is also a vector of the same length as
elementTypes
; each entry is a vector of length equal to the number of
elements of the given type times the number N of nodes for this type of element,
that contains the node tags of all the elements of the given type, concatenated:
[e1n1, e1n2, ..., e1nN, e2n1, ...].
dim = -1
, tag = -1
elementTypes
, elementTags
, nodeTags
-
C++ (x1.cpp, adapt_mesh.cpp, explore.cpp), Python (x1.py, copy_mesh.py, explore.py, flatten.py, test.py)
gmsh/model/mesh/getElement
¶Get the type and node tags of the element with tag tag
. This function
relies on an internal cache (a vector in case of dense element numbering, a map
otherwise); for large meshes accessing elements in bulk is often preferable.
gmsh/model/mesh/getElementByCoordinates
¶Search the mesh for an element located at coordinates (x
, y
,
z
). This function performs a search in a spatial octree. If an element is
found, return its tag, type and node tags, as well as the local coordinates
(u
, v
, w
) within the reference element corresponding to
search location. If dim
is >= 0, only search for elements of the given
dimension. If strict
is not set, use a tolerance to find elements near
the search location.
gmsh/model/mesh/getElementsByCoordinates
¶Search the mesh for element(s) located at coordinates (x
, y
,
z
). This function performs a search in a spatial octree. Return the tags
of all found elements in elementTags
. Additional information about the
elements can be accessed through getElement
and
getLocalCoordinatesInElement
. If dim
is >= 0, only search for
elements of the given dimension. If strict
is not set, use a tolerance to
find elements near the search location.
gmsh/model/mesh/getLocalCoordinatesInElement
¶Return the local coordinates (u
, v
, w
) within the element
elementTag
corresponding to the model coordinates (x
, y
,
z
). This function relies on an internal cache (a vector in case of dense
element numbering, a map otherwise); for large meshes accessing elements in bulk
is often preferable.
gmsh/model/mesh/getElementTypes
¶Get the types of elements in the entity of dimension dim
and tag
tag
. If tag
< 0, get the types for all entities of dimension
dim
. If dim
and tag
are negative, get all the types in the
mesh.
gmsh/model/mesh/getElementType
¶Return an element type given its family name familyName
("Point", "Line",
"Triangle", "Quadrangle", "Tetrahedron", "Pyramid", "Prism", "Hexahedron") and
polynomial order order
. If serendip
is true, return the
corresponding serendip element type (element without interior nodes).
gmsh/model/mesh/getElementProperties
¶Get the properties of an element of type elementType
: its name
(elementName
), dimension (dim
), order (order
), number of
nodes (numNodes
), local coordinates of the nodes in the reference element
(localNodeCoord
vector, of length dim
times numNodes
) and
number of primary (first order) nodes (numPrimaryNodes
).
elementType
elementName
, dim
, order
, numNodes
, localNodeCoord
, numPrimaryNodes
-
C++ (x1.cpp, edges.cpp, explore.cpp, faces.cpp), Python (x1.py, explore.py, poisson.py)
gmsh/model/mesh/getElementsByType
¶Get the elements of type elementType
classified on the entity of tag
tag
. If tag
< 0, get the elements for all entities.
elementTags
is a vector containing the tags (unique, strictly positive
identifiers) of the elements of the corresponding type. nodeTags
is a
vector of length equal to the number of elements of the given type times the
number N of nodes for this type of element, that contains the node tags of all
the elements of the given type, concatenated: [e1n1, e1n2, ..., e1nN, e2n1,
...]. If numTasks
> 1, only compute and return the part of the data
indexed by task
.
elementType
, tag = -1
, task = 0
, numTasks = 1
elementTags
, nodeTags
-
C++ (edges.cpp, faces.cpp), Python (adapt_mesh.py, neighbors.py, poisson.py)
gmsh/model/mesh/preallocateElementsByType
¶Preallocate data before calling getElementsByType
with numTasks
>
1. For C and C++ only.
gmsh/model/mesh/addElements
¶Add elements classified on the entity of dimension dim
and tag
tag
. types
contains the MSH types of the elements (e.g. 2
for 3-node triangles: see the Gmsh reference manual). elementTags
is a
vector of the same length as types
; each entry is a vector containing the
tags (unique, strictly positive identifiers) of the elements of the
corresponding type. nodeTags
is also a vector of the same length as
types
; each entry is a vector of length equal to the number of elements
of the given type times the number N of nodes per element, that contains the
node tags of all the elements of the given type, concatenated: [e1n1, e1n2, ...,
e1nN, e2n1, ...].
dim
, tag
, elementTypes
, elementTags
, nodeTags
-
-
C++ (discrete.cpp, plugin.cpp, view.cpp), Python (copy_mesh.py, discrete.py, flatten.py, mesh_from_discrete_curve.py, plugin.py, ...)
gmsh/model/mesh/addElementsByType
¶Add elements of type elementType
classified on the entity of tag
tag
. elementTags
contains the tags (unique, strictly positive
identifiers) of the elements of the corresponding type. nodeTags
is a
vector of length equal to the number of elements times the number N of nodes per
element, that contains the node tags of all the elements, concatenated: [e1n1,
e1n2, ..., e1nN, e2n1, ...]. If the elementTag
vector is empty, new tags
are automatically assigned to the elements.
tag
, elementType
, elementTags
, nodeTags
-
-
C++ (x2.cpp, x4.cpp, edges.cpp, faces.cpp, import_perf.cpp), Python (x2.py, x4.py, import_perf.py, raw_tetrahedralization.py, raw_triangulation.py, ...)
gmsh/model/mesh/getIntegrationPoints
¶Get the numerical quadrature information for the given element type
elementType
and integration rule integrationType
(e.g. "Gauss4"
for a Gauss quadrature suited for integrating 4th order polynomials).
localCoord
contains the u, v, w coordinates of the G integration points
in the reference element: [g1u, g1v, g1w, ..., gGu, gGv, gGw]. weights
contains the associated weights: [g1q, ..., gGq].
elementType
, integrationType
localCoord
, weights
-
C++ (adapt_mesh.cpp, edges.cpp, faces.cpp), Python (adapt_mesh.py, poisson.py)
gmsh/model/mesh/getJacobians
¶Get the Jacobians of all the elements of type elementType
classified on
the entity of tag tag
, at the G evaluation points localCoord
given
as concatenated triplets of coordinates in the reference element [g1u, g1v, g1w,
..., gGu, gGv, gGw]. Data is returned by element, with elements in the same
order as in getElements
and getElementsByType
. jacobians
contains for each element the 9 entries of the 3x3 Jacobian matrix at each
evaluation point. The matrix is returned by column: [e1g1Jxu, e1g1Jyu, e1g1Jzu,
e1g1Jxv, ..., e1g1Jzw, e1g2Jxu, ..., e1gGJzw, e2g1Jxu, ...], with Jxu=dx/du,
Jyu=dy/du, etc. determinants
contains for each element the determinant of
the Jacobian matrix at each evaluation point: [e1g1, e1g2, ... e1gG, e2g1, ...].
coord
contains for each element the x, y, z coordinates of the evaluation
points. If tag
< 0, get the Jacobian data for all entities. If
numTasks
> 1, only compute and return the part of the data indexed by
task
.
elementType
, localCoord
, tag = -1
, task = 0
, numTasks = 1
jacobians
, determinants
, coord
-
C++ (adapt_mesh.cpp, edges.cpp, faces.cpp), Python (adapt_mesh.py, poisson.py)
gmsh/model/mesh/preallocateJacobians
¶Preallocate data before calling getJacobians
with numTasks
> 1.
For C and C++ only.
gmsh/model/mesh/getJacobian
¶Get the Jacobian for a single element elementTag
, at the G evaluation
points localCoord
given as concatenated triplets of coordinates in the
reference element [g1u, g1v, g1w, ..., gGu, gGv, gGw]. jacobians
contains
the 9 entries of the 3x3 Jacobian matrix at each evaluation point. The matrix is
returned by column: [e1g1Jxu, e1g1Jyu, e1g1Jzu, e1g1Jxv, ..., e1g1Jzw, e1g2Jxu,
..., e1gGJzw, e2g1Jxu, ...], with Jxu=dx/du, Jyu=dy/du, etc. determinants
contains the determinant of the Jacobian matrix at each evaluation point.
coord
contains the x, y, z coordinates of the evaluation points. This
function relies on an internal cache (a vector in case of dense element
numbering, a map otherwise); for large meshes accessing Jacobians in bulk is
often preferable.
gmsh/model/mesh/getBasisFunctions
¶Get the basis functions of the element of type elementType
at the
evaluation points localCoord
(given as concatenated triplets of
coordinates in the reference element [g1u, g1v, g1w, ..., gGu, gGv, gGw]), for
the function space functionSpaceType
(e.g. "Lagrange" or "GradLagrange"
for Lagrange basis functions or their gradient, in the u, v, w coordinates of
the reference element; or "H1Legendre3" or "GradH1Legendre3" for 3rd order
hierarchical H1 Legendre functions). numComponents
returns the number C
of components of a basis function. basisFunctions
returns the value of
the N basis functions at the evaluation points, i.e. [g1f1, g1f2, ..., g1fN,
g2f1, ...] when C == 1 or [g1f1u, g1f1v, g1f1w, g1f2u, ..., g1fNw, g2f1u, ...]
when C == 3. For basis functions that depend on the orientation of the elements,
all values for the first orientation are returned first, followed by values for
the second, etc. numOrientations
returns the overall number of
orientations. If wantedOrientations
is not empty, only return the values
for the desired orientation indices.
elementType
, localCoord
, functionSpaceType
, wantedOrientations = []
numComponents
, basisFunctions
, numOrientations
-
C++ (edges.cpp, faces.cpp), Python (adapt_mesh.py, poisson.py)
gmsh/model/mesh/getBasisFunctionsOrientationForElements
¶Get the orientation index of the elements of type elementType
in the
entity of tag tag
. The arguments have the same meaning as in
getBasisFunctions
. basisFunctionsOrientation
is a vector giving
for each element the orientation index in the values returned by
getBasisFunctions
. For Lagrange basis functions the call is superfluous
as it will return a vector of zeros.
gmsh/model/mesh/getBasisFunctionsOrientationForElement
¶Get the orientation of a single element elementTag
.
gmsh/model/mesh/getNumberOfOrientations
¶Get the number of possible orientations for elements of type elementType
and function space named functionSpaceType
.
gmsh/model/mesh/preallocateBasisFunctionsOrientationForElements
¶Preallocate data before calling getBasisFunctionsOrientationForElements
with numTasks
> 1. For C and C++ only.
gmsh/model/mesh/getEdges
¶Get the global unique mesh edge identifiers edgeTags
and orientations
edgeOrientation
for an input list of node tag pairs defining these edges,
concatenated in the vector nodeTags
.
gmsh/model/mesh/getFaces
¶Get the global unique mesh face identifiers faceTags
and orientations
faceOrientations
for an input list of node tag triplets (if
faceType
== 3) or quadruplets (if faceType
== 4) defining these
faces, concatenated in the vector nodeTags
.
gmsh/model/mesh/createEdges
¶Create unique mesh edges for the entities dimTags
.
gmsh/model/mesh/createFaces
¶Create unique mesh faces for the entities dimTags
.
gmsh/model/mesh/getLocalMultipliersForHcurl0
¶Get the local multipliers (to guarantee H(curl)-conformity) of the order 0 H(curl) basis functions. Warning: this is an experimental feature and will probably change in a future release.
gmsh/model/mesh/getKeysForElements
¶Generate the keys
for the elements of type elementType
in the
entity of tag tag
, for the functionSpaceType
function space. Each
key uniquely identifies a basis function in the function space. If
returnCoord
is set, the coord
vector contains the x, y, z
coordinates locating basis functions for sorting purposes. Warning: this is an
experimental feature and will probably change in a future release.
gmsh/model/mesh/getKeysForElement
¶Get the keys for a single element elementTag
.
gmsh/model/mesh/getNumberOfKeysForElements
¶Get the number of keys by elements of type elementType
for function space
named functionSpaceType
.
gmsh/model/mesh/getInformationForElements
¶Get information about the keys
. infoKeys
returns information about
the functions associated with the keys
. infoKeys[0].first
describes the type of function (0 for vertex function, 1 for edge function, 2
for face function and 3 for bubble function). infoKeys[0].second
gives
the order of the function associated with the key. Warning: this is an
experimental feature and will probably change in a future release.
gmsh/model/mesh/getBarycenters
¶Get the barycenters of all elements of type elementType
classified on the
entity of tag tag
. If primary
is set, only the primary nodes of
the elements are taken into account for the barycenter calculation. If
fast
is set, the function returns the sum of the primary node coordinates
(without normalizing by the number of nodes). If tag
< 0, get the
barycenters for all entities. If numTasks
> 1, only compute and return
the part of the data indexed by task
.
gmsh/model/mesh/preallocateBarycenters
¶Preallocate data before calling getBarycenters
with numTasks
> 1.
For C and C++ only.
gmsh/model/mesh/getElementEdgeNodes
¶Get the nodes on the edges of all elements of type elementType
classified
on the entity of tag tag
. nodeTags
contains the node tags of the
edges for all the elements: [e1a1n1, e1a1n2, e1a2n1, ...]. Data is returned by
element, with elements in the same order as in getElements
and
getElementsByType
. If primary
is set, only the primary (begin/end)
nodes of the edges are returned. If tag
< 0, get the edge nodes for all
entities. If numTasks
> 1, only compute and return the part of the data
indexed by task
.
gmsh/model/mesh/getElementFaceNodes
¶Get the nodes on the faces of type faceType
(3 for triangular faces, 4
for quadrangular faces) of all elements of type elementType
classified on
the entity of tag tag
. nodeTags
contains the node tags of the
faces for all elements: [e1f1n1, ..., e1f1nFaceType, e1f2n1, ...]. Data is
returned by element, with elements in the same order as in getElements
and getElementsByType
. If primary
is set, only the primary
(corner) nodes of the faces are returned. If tag
< 0, get the face nodes
for all entities. If numTasks
> 1, only compute and return the part of
the data indexed by task
.
gmsh/model/mesh/getGhostElements
¶Get the ghost elements elementTags
and their associated partitions
stored in the ghost entity of dimension dim
and tag tag
.
gmsh/model/mesh/setSize
¶Set a mesh size constraint on the model entities dimTags
. Currently only
entities of dimension 0 (points) are handled.
dimTags
, size
-
-
C++ (t16.cpp, t18.cpp, t21.cpp, adapt_mesh.cpp), Python (t16.py, t18.py, t21.py, adapt_mesh.py, periodic.py, ...)
gmsh/model/mesh/setSizeAtParametricPoints
¶Set mesh size constraints at the given parametric points parametricCoord
on the model entity of dimension dim
and tag tag
. Currently only
entities of dimension 1 (lines) are handled.
gmsh/model/mesh/setSizeCallback
¶Set a global mesh size callback. The callback should take 5 arguments
(dim
, tag
, x
, y
and z
) and return the value
of the mesh size at coordinates (x
, y
, z
).
gmsh/model/mesh/removeSizeCallback
¶Remove the global mesh size callback.
gmsh/model/mesh/setTransfiniteCurve
¶Set a transfinite meshing constraint on the curve tag
, with
numNodes
nodes distributed according to meshType
and coef
.
Currently supported types are "Progression" (geometrical progression with power
coef
), "Bump" (refinement toward both extremities of the curve) and
"Beta" (beta law).
tag
, numNodes
, meshType = "Progression"
, coef = 1.
-
-
C++ (x2.cpp), Python (x2.py, terrain.py, terrain_bspline.py, terrain_stl.py)
gmsh/model/mesh/setTransfiniteSurface
¶Set a transfinite meshing constraint on the surface tag
.
arrangement
describes the arrangement of the triangles when the surface
is not flagged as recombined: currently supported values are "Left", "Right",
"AlternateLeft" and "AlternateRight". cornerTags
can be used to specify
the (3 or 4) corners of the transfinite interpolation explicitly; specifying the
corners explicitly is mandatory if the surface has more that 3 or 4 points on
its boundary.
tag
, arrangement = "Left"
, cornerTags = []
-
-
C++ (x2.cpp, get_data_perf.cpp, square.cpp), Python (x2.py, get_data_perf.py, terrain.py, terrain_bspline.py, terrain_stl.py)
gmsh/model/mesh/setTransfiniteVolume
¶Set a transfinite meshing constraint on the surface tag
.
cornerTags
can be used to specify the (6 or 8) corners of the transfinite
interpolation explicitly.
tag
, cornerTags = []
-
-
C++ (x2.cpp), Python (x2.py, terrain.py, terrain_bspline.py, terrain_stl.py)
gmsh/model/mesh/setTransfiniteAutomatic
¶Set transfinite meshing constraints on the model entities in dimTag
.
Transfinite meshing constraints are added to the curves of the quadrangular
surfaces and to the faces of 6-sided volumes. Quadragular faces with a corner
angle superior to cornerAngle
(in radians) are ignored. The number of
points is automatically determined from the sizing constraints. If dimTag
is empty, the constraints are applied to all entities in the model. If
recombine
is true, the recombine flag is automatically set on the
transfinite surfaces.
gmsh/model/mesh/setRecombine
¶Set a recombination meshing constraint on the model entity of dimension
dim
and tag tag
. Currently only entities of dimension 2 (to
recombine triangles into quadrangles) are supported.
dim
, tag
-
-
C++ (t11.cpp, x2.cpp), Python (t11.py, x2.py, poisson.py, terrain.py, terrain_bspline.py, ...)
gmsh/model/mesh/setSmoothing
¶Set a smoothing meshing constraint on the model entity of dimension dim
and tag tag
. val
iterations of a Laplace smoother are applied.
dim
, tag
, val
-
-
C++ (x2.cpp), Python (x2.py, terrain.py, terrain_bspline.py, terrain_stl.py)
gmsh/model/mesh/setReverse
¶Set a reverse meshing constraint on the model entity of dimension dim
and
tag tag
. If val
is true, the mesh orientation will be reversed
with respect to the natural mesh orientation (i.e. the orientation consistent
with the orientation of the geometry). If val
is false, the mesh is left
as-is.
gmsh/model/mesh/setAlgorithm
¶Set the meshing algorithm on the model entity of dimension dim
and tag
tag
. Currently only supported for dim
== 2.
gmsh/model/mesh/setSizeFromBoundary
¶Force the mesh size to be extended from the boundary, or not, for the model
entity of dimension dim
and tag tag
. Currently only supported for
dim
== 2.
gmsh/model/mesh/setCompound
¶Set a compound meshing constraint on the model entities of dimension dim
and tags tags
. During meshing, compound entities are treated as a single
discrete entity, which is automatically reparametrized.
gmsh/model/mesh/setOutwardOrientation
¶Set meshing constraints on the bounding surfaces of the volume of tag tag
so that all surfaces are oriented with outward pointing normals. Currently only
available with the OpenCASCADE kernel, as it relies on the STL triangulation.
gmsh/model/mesh/removeConstraints
¶Remove all meshing constraints from the model entities dimTags
. If
dimTags
is empty, remove all constraings.
dimTags = []
-
-
Python (terrain_bspline.py)
gmsh/model/mesh/embed
¶Embed the model entities of dimension dim
and tags tags
in the
(inDim
, inTag
) model entity. The dimension dim
can 0, 1 or
2 and must be strictly smaller than inDim
, which must be either 2 or 3.
The embedded entities should not intersect each other or be part of the boundary
of the entity inTag
, whose mesh will conform to the mesh of the embedded
entities. With the OpenCASCADE kernel, if the fragment
operation is
applied to entities of different dimensions, the lower dimensional entities will
be automatically embedded in the higher dimensional entities if they are not on
their boundary.
gmsh/model/mesh/removeEmbedded
¶Remove embedded entities from the model entities dimTags
. if dim
is >= 0, only remove embedded entities of the given dimension (e.g. embedded
points if dim
== 0).
gmsh/model/mesh/getEmbedded
¶Get the entities (if any) embedded in the model entity of dimension dim
and tag tag
.
gmsh/model/mesh/reorderElements
¶Reorder the elements of type elementType
classified on the entity of tag
tag
according to ordering
.
gmsh/model/mesh/renumberNodes
¶Renumber the node tags in a continuous sequence.
gmsh/model/mesh/renumberElements
¶Renumber the element tags in a continuous sequence.
gmsh/model/mesh/setPeriodic
¶Set the meshes of the entities of dimension dim
and tag tags
as
periodic copies of the meshes of entities tagsMaster
, using the affine
transformation specified in affineTransformation
(16 entries of a 4x4
matrix, by row). If used after meshing, generate the periodic node
correspondence information assuming the meshes of entities tags
effectively match the meshes of entities tagsMaster
(useful for
structured and extruded meshes). Currently only available for dim
== 1
and dim
== 2.
gmsh/model/mesh/getPeriodicNodes
¶Get the master entity tagMaster
, the node tags nodeTags
and their
corresponding master node tags nodeTagsMaster
, and the affine transform
affineTransform
for the entity of dimension dim
and tag
tag
. If includeHighOrderNodes
is set, include high-order nodes in
the returned data.
dim
, tag
, includeHighOrderNodes = False
tagMaster
, nodeTags
, nodeTagsMaster
, affineTransform
-
Python (periodic.py)
gmsh/model/mesh/removeDuplicateNodes
¶Remove duplicate nodes in the mesh of the current model.
-
-
-
Python (glue_and_remesh_stl.py)
gmsh/model/mesh/splitQuadrangles
¶Split (into two triangles) all quadrangles in surface tag
whose quality
is lower than quality
. If tag
< 0, split quadrangles in all
surfaces.
gmsh/model/mesh/classifySurfaces
¶Classify ("color") the surface mesh based on the angle threshold angle
(in radians), and create new discrete surfaces, curves and points accordingly.
If boundary
is set, also create discrete curves on the boundary if the
surface is open. If forReparametrization
is set, create edges and
surfaces that can be reparametrized using a single map. If curveAngle
is
less than Pi, also force curves to be split according to curveAngle
. If
exportDiscrete
is set, clear any built-in CAD kernel entities and export
the discrete entities in the built-in CAD kernel.
angle
, boundary = True
, forReparametrization = False
, curveAngle = pi
, exportDiscrete = True
-
-
C++ (t13.cpp), Python (t13.py, aneurysm.py, glue_and_remesh_stl.py, remesh_stl.py, terrain_stl.py)
gmsh/model/mesh/createGeometry
¶Create a geometry for the discrete entities dimTags
(represented solely
by a mesh, without an underlying CAD description), i.e. create a parametrization
for discrete curves and surfaces, assuming that each can be parametrized with a
single map. If dimTags
is empty, create a geometry for all the discrete
entities.
dimTags = []
-
-
C++ (t13.cpp, x2.cpp), Python (t13.py, x2.py, aneurysm.py, glue_and_remesh_stl.py, remesh_stl.py, ...)
gmsh/model/mesh/createTopology
¶Create a boundary representation from the mesh if the model does not have one
(e.g. when imported from mesh file formats with no BRep representation of the
underlying model). If makeSimplyConnected
is set, enforce simply
connected discrete surfaces and volumes. If exportDiscrete
is set, clear
any built-in CAD kernel entities and export the discrete entities in the built-
in CAD kernel.
gmsh/model/mesh/computeHomology
¶Compute a basis representation for homology spaces after a mesh has been
generated. The computation domain is given in a list of physical group tags
domainTags
; if empty, the whole mesh is the domain. The computation
subdomain for relative homology computation is given in a list of physical group
tags subdomainTags
; if empty, absolute homology is computed. The
dimensions homology bases to be computed are given in the list dim
; if
empty, all bases are computed. Resulting basis representation chains are stored
as physical groups in the mesh.
gmsh/model/mesh/computeCohomology
¶Compute a basis representation for cohomology spaces after a mesh has been
generated. The computation domain is given in a list of physical group tags
domainTags
; if empty, the whole mesh is the domain. The computation
subdomain for relative cohomology computation is given in a list of physical
group tags subdomainTags
; if empty, absolute cohomology is computed. The
dimensions homology bases to be computed are given in the list dim
; if
empty, all bases are computed. Resulting basis representation cochains are
stored as physical groups in the mesh.
gmsh/model/mesh/computeCrossField
¶Compute a cross field for the current mesh. The function creates 3 views: the H function, the Theta function and cross directions. Return the tags of the views.
gmsh/model/mesh/triangulate
¶Triangulate the points given in the coord
vector as pairs of u, v
coordinates, and return the node tags (with numbering starting at 1) of the
resulting triangles in tri
.
coord
tri
-
Python (raw_triangulation.py)
gmsh/model/mesh/tetrahedralize
¶Tetrahedralize the points given in the coord
vector as triplets of x, y,
z coordinates, and return the node tags (with numbering starting at 1) of the
resulting tetrahedra in tetra
.
coord
tetra
-
Python (raw_tetrahedralization.py)
Next: Namespace gmsh/model/geo
: built-in CAD kernel functions, Previous: Namespace gmsh/model/mesh
: mesh functions, Up: Gmsh API [Contents][Index]
gmsh/model/mesh/field
: mesh size field functionsgmsh/model/mesh/field/add
¶Add a new mesh size field of type fieldType
. If tag
is positive,
assign the tag explicitly; otherwise a new tag is assigned automatically. Return
the field tag.
gmsh/model/mesh/field/remove
¶Remove the field with tag tag
.
gmsh/model/mesh/field/setNumber
¶Set the numerical option option
to value value
for field
tag
.
tag
, option
, value
-
-
C++ (t7.cpp, t10.cpp, t17.cpp, adapt_mesh.cpp), Python (t7.py, t10.py, t17.py, adapt_mesh.py, copy_mesh.py)
gmsh/model/mesh/field/setString
¶Set the string option option
to value value
for field tag
.
gmsh/model/mesh/field/setNumbers
¶Set the numerical list option option
to value value
for field
tag
.
gmsh/model/mesh/field/setAsBackgroundMesh
¶Set the field tag
as the background mesh size field.
gmsh/model/mesh/field/setAsBoundaryLayer
¶Set the field tag
as a boundary layer size field.
Next: Namespace gmsh/model/geo/mesh
: built-in CAD kernel meshing constraints, Previous: Namespace gmsh/model/mesh/field
: mesh size field functions, Up: Gmsh API [Contents][Index]
gmsh/model/geo
: built-in CAD kernel functionsgmsh/model/geo/addPoint
¶Add a geometrical point in the built-in CAD representation, at coordinates
(x
, y
, z
). If meshSize
is > 0, add a meshing
constraint at that point. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. Return the tag of the point.
(Note that the point will be added in the current model only after
synchronize
is called. This behavior holds for all the entities added in
the geo module.)
gmsh/model/geo/addLine
¶Add a straight line segment in the built-in CAD representation, between the two
points with tags startTag
and endTag
. If tag
is positive,
set the tag explicitly; otherwise a new tag is selected automatically. Return
the tag of the line.
gmsh/model/geo/addCircleArc
¶Add a circle arc (strictly smaller than Pi) in the built-in CAD representation,
between the two points with tags startTag
and endTag
, and with
center centerTag
. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. If (nx
, ny
,
nz
) != (0, 0, 0), explicitly set the plane of the circle arc. Return the
tag of the circle arc.
gmsh/model/geo/addEllipseArc
¶Add an ellipse arc (strictly smaller than Pi) in the built-in CAD
representation, between the two points startTag
and endTag
, and
with center centerTag
and major axis point majorTag
. If tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. If (nx
, ny
, nz
) != (0, 0, 0), explicitly set
the plane of the circle arc. Return the tag of the ellipse arc.
gmsh/model/geo/addSpline
¶Add a spline (Catmull-Rom) curve in the built-in CAD representation, going
through the points pointTags
. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Create a periodic
curve if the first and last points are the same. Return the tag of the spline
curve.
gmsh/model/geo/addBSpline
¶Add a cubic b-spline curve in the built-in CAD representation, with
pointTags
control points. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Creates a periodic
curve if the first and last points are the same. Return the tag of the b-spline
curve.
gmsh/model/geo/addBezier
¶Add a Bezier curve in the built-in CAD representation, with pointTags
control points. If tag
is positive, set the tag explicitly; otherwise a
new tag is selected automatically. Return the tag of the Bezier curve.
gmsh/model/geo/addPolyline
¶Add a polyline curve in the built-in CAD representation, going through the
points pointTags
. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. Create a periodic curve if the
first and last points are the same. Return the tag of the polyline curve.
gmsh/model/geo/addCompoundSpline
¶Add a spline (Catmull-Rom) curve in the built-in CAD representation, going
through points sampling the curves in curveTags
. The density of sampling
points on each curve is governed by numIntervals
. If tag
is
positive, set the tag explicitly; otherwise a new tag is selected automatically.
Return the tag of the spline.
gmsh/model/geo/addCompoundBSpline
¶Add a b-spline curve in the built-in CAD representation, with control points
sampling the curves in curveTags
. The density of sampling points on each
curve is governed by numIntervals
. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Return the tag of the
b-spline.
gmsh/model/geo/addCurveLoop
¶Add a curve loop (a closed wire) in the built-in CAD representation, formed by
the curves curveTags
. curveTags
should contain (signed) tags of
model entities of dimension 1 forming a closed loop: a negative tag signifies
that the underlying curve is considered with reversed orientation. If tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. If reorient
is set, automatically reorient the curves if
necessary. Return the tag of the curve loop.
gmsh/model/geo/addCurveLoops
¶Add curve loops in the built-in CAD representation based on the curves
curveTags
. Return the tags
of found curve loops, if any.
curveTags
tags
-
Python (aneurysm.py)
gmsh/model/geo/addPlaneSurface
¶Add a plane surface in the built-in CAD representation, defined by one or more
curve loops wireTags
. The first curve loop defines the exterior contour;
additional curve loop define holes. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Return the tag of the
surface.
gmsh/model/geo/addSurfaceFilling
¶Add a surface in the built-in CAD representation, filling the curve loops in
wireTags
using transfinite interpolation. Currently only a single curve
loop is supported; this curve loop should be composed by 3 or 4 curves only. If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the surface.
gmsh/model/geo/addSurfaceLoop
¶Add a surface loop (a closed shell) formed by surfaceTags
in the built-in
CAD representation. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. Return the tag of the shell.
gmsh/model/geo/addVolume
¶Add a volume (a region) in the built-in CAD representation, defined by one or
more shells shellTags
. The first surface loop defines the exterior
boundary; additional surface loop define holes. If tag
is positive, set
the tag explicitly; otherwise a new tag is selected automatically. Return the
tag of the volume.
gmsh/model/geo/extrude
¶Extrude the entities dimTags
in the built-in CAD representation, using a
translation along (dx
, dy
, dz
). Return extruded entities in
outDimTags
. If numElements
is not empty, also extrude the mesh:
the entries in numElements
give the number of elements in each layer. If
height
is not empty, it provides the (cumulative) height of the different
layers, normalized to 1. If recombine
is set, recombine the mesh in the
layers.
gmsh/model/geo/revolve
¶Extrude the entities dimTags
in the built-in CAD representation, using a
rotation of angle
radians around the axis of revolution defined by the
point (x
, y
, z
) and the direction (ax
, ay
,
az
). The angle should be strictly smaller than Pi. Return extruded
entities in outDimTags
. If numElements
is not empty, also extrude
the mesh: the entries in numElements
give the number of elements in each
layer. If height
is not empty, it provides the (cumulative) height of the
different layers, normalized to 1. If recombine
is set, recombine the
mesh in the layers.
gmsh/model/geo/twist
¶Extrude the entities dimTags
in the built-in CAD representation, using a
combined translation and rotation of angle
radians, along (dx
,
dy
, dz
) and around the axis of revolution defined by the point
(x
, y
, z
) and the direction (ax
, ay
,
az
). The angle should be strictly smaller than Pi. Return extruded
entities in outDimTags
. If numElements
is not empty, also extrude
the mesh: the entries in numElements
give the number of elements in each
layer. If height
is not empty, it provides the (cumulative) height of the
different layers, normalized to 1. If recombine
is set, recombine the
mesh in the layers.
gmsh/model/geo/extrudeBoundaryLayer
¶Extrude the entities dimTags
in the built-in CAD representation along the
normals of the mesh, creating discrete boundary layer entities. Return extruded
entities in outDimTags
. The entries in numElements
give the number
of elements in each layer. If height
is not empty, it provides the height
of the different layers. If recombine
is set, recombine the mesh in the
layers. A second boundary layer can be created from the same entities if
second
is set. If viewIndex
is >= 0, use the corresponding view to
either specify the normals (if the view contains a vector field) or scale the
normals (if the view is scalar).
dimTags
, numElements = [1]
, heights = []
, recombine = False
, second = False
, viewIndex = -1
outDimTags
-
Python (aneurysm.py)
gmsh/model/geo/translate
¶Translate the entities dimTags
in the built-in CAD representation along
(dx
, dy
, dz
).
gmsh/model/geo/rotate
¶Rotate the entities dimTags
in the built-in CAD representation by
angle
radians around the axis of revolution defined by the point
(x
, y
, z
) and the direction (ax
, ay
,
az
).
gmsh/model/geo/dilate
¶Scale the entities dimTag
in the built-in CAD representation by factors
a
, b
and c
along the three coordinate axes; use (x
,
y
, z
) as the center of the homothetic transformation.
gmsh/model/geo/mirror
¶Mirror the entities dimTag
in the built-in CAD representation, with
respect to the plane of equation a
* x + b
* y + c
* z +
d
= 0.
gmsh/model/geo/symmetrize
¶Mirror the entities dimTag
in the built-in CAD representation, with
respect to the plane of equation a
* x + b
* y + c
* z +
d
= 0. (This is a synonym for mirror
, which will be deprecated in
a future release.)
gmsh/model/geo/copy
¶Copy the entities dimTags
in the built-in CAD representation; the new
entities are returned in outDimTags
.
gmsh/model/geo/remove
¶Remove the entities dimTags
in the built-in CAD representation. If
recursive
is true, remove all the entities on their boundaries, down to
dimension 0.
gmsh/model/geo/removeAllDuplicates
¶Remove all duplicate entities in the built-in CAD representation (different entities at the same geometrical location).
gmsh/model/geo/splitCurve
¶Split the curve of tag tag
in the built-in CAD representation, on the
control points pointTags
. Return the tags curveTags
of the newly
created curves.
gmsh/model/geo/getMaxTag
¶Get the maximum tag of entities of dimension dim
in the built-in CAD
representation.
gmsh/model/geo/setMaxTag
¶Set the maximum tag maxTag
for entities of dimension dim
in the
built-in CAD representation.
gmsh/model/geo/addPhysicalGroup
¶Add a physical group of dimension dim
, grouping the entities with tags
tags
in the built-in CAD representation. Return the tag of the physical
group, equal to tag
if tag
is positive, or a new tag if tag
< 0.
gmsh/model/geo/removePhysicalGroups
¶Remove the physical groups dimTags
from the built-in CAD representation.
If dimTags
is empty, remove all groups.
gmsh/model/geo/synchronize
¶Synchronize the built-in CAD representation with the current Gmsh model. This can be called at any time, but since it involves a non trivial amount of processing, the number of synchronization points should normally be minimized. Without synchronization the entities in the built-in CAD representation are not available to any function outside of the built-in CAD kernel functions.
Next: Namespace gmsh/model/occ
: OpenCASCADE CAD kernel functions, Previous: Namespace gmsh/model/geo
: built-in CAD kernel functions, Up: Gmsh API [Contents][Index]
gmsh/model/geo/mesh
: built-in CAD kernel meshing constraintsgmsh/model/geo/mesh/setSize
¶Set a mesh size constraint on the entities dimTags
in the built-in CAD
kernel representation. Currently only entities of dimension 0 (points) are
handled.
gmsh/model/geo/mesh/setTransfiniteCurve
¶Set a transfinite meshing constraint on the curve tag
in the built-in CAD
kernel representation, with numNodes
nodes distributed according to
meshType
and coef
. Currently supported types are "Progression"
(geometrical progression with power coef
) and "Bump" (refinement toward
both extremities of the curve).
gmsh/model/geo/mesh/setTransfiniteSurface
¶Set a transfinite meshing constraint on the surface tag
in the built-in
CAD kernel representation. arrangement
describes the arrangement of the
triangles when the surface is not flagged as recombined: currently supported
values are "Left", "Right", "AlternateLeft" and "AlternateRight".
cornerTags
can be used to specify the (3 or 4) corners of the transfinite
interpolation explicitly; specifying the corners explicitly is mandatory if the
surface has more that 3 or 4 points on its boundary.
gmsh/model/geo/mesh/setTransfiniteVolume
¶Set a transfinite meshing constraint on the surface tag
in the built-in
CAD kernel representation. cornerTags
can be used to specify the (6 or 8)
corners of the transfinite interpolation explicitly.
gmsh/model/geo/mesh/setRecombine
¶Set a recombination meshing constraint on the entity of dimension dim
and
tag tag
in the built-in CAD kernel representation. Currently only
entities of dimension 2 (to recombine triangles into quadrangles) are supported.
gmsh/model/geo/mesh/setSmoothing
¶Set a smoothing meshing constraint on the entity of dimension dim
and tag
tag
in the built-in CAD kernel representation. val
iterations of a
Laplace smoother are applied.
gmsh/model/geo/mesh/setReverse
¶Set a reverse meshing constraint on the entity of dimension dim
and tag
tag
in the built-in CAD kernel representation. If val
is true, the
mesh orientation will be reversed with respect to the natural mesh orientation
(i.e. the orientation consistent with the orientation of the geometry). If
val
is false, the mesh is left as-is.
gmsh/model/geo/mesh/setAlgorithm
¶Set the meshing algorithm on the entity of dimension dim
and tag
tag
in the built-in CAD kernel representation. Currently only supported
for dim
== 2.
gmsh/model/geo/mesh/setSizeFromBoundary
¶Force the mesh size to be extended from the boundary, or not, for the entity of
dimension dim
and tag tag
in the built-in CAD kernel
representation. Currently only supported for dim
== 2.
Next: Namespace gmsh/model/occ/mesh
: OpenCASCADE CAD kernel meshing constraints, Previous: Namespace gmsh/model/geo/mesh
: built-in CAD kernel meshing constraints, Up: Gmsh API [Contents][Index]
gmsh/model/occ
: OpenCASCADE CAD kernel functionsgmsh/model/occ/addPoint
¶Add a geometrical point in the OpenCASCADE CAD representation, at coordinates
(x
, y
, z
). If meshSize
is > 0, add a meshing
constraint at that point. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. Return the tag of the point.
(Note that the point will be added in the current model only after
synchronize
is called. This behavior holds for all the entities added in
the occ module.)
x
, y
, z
, meshSize = 0.
, tag = -1
-
integer value
C++ (t19.cpp, spline.cpp), Python (t19.py, bspline_bezier_patches.py, bspline_bezier_trimmed.py, bspline_filling.py, closest_point.py, ...)
gmsh/model/occ/addLine
¶Add a straight line segment in the OpenCASCADE CAD representation, between the
two points with tags startTag
and endTag
. If tag
is
positive, set the tag explicitly; otherwise a new tag is selected automatically.
Return the tag of the line.
gmsh/model/occ/addCircleArc
¶Add a circle arc in the OpenCASCADE CAD representation, between the two points
with tags startTag
and endTag
, with center centerTag
. If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the circle arc.
gmsh/model/occ/addCircle
¶Add a circle of center (x
, y
, z
) and radius r
in the
OpenCASCADE CAD representation. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. If angle1
and
angle2
are specified, create a circle arc between the two angles. Return
the tag of the circle.
x
, y
, z
, r
, tag = -1
, angle1 = 0.
, angle2 = 2*pi
-
integer value
C++ (t19.cpp), Python (t19.py, bspline_bezier_trimmed.py, closest_point.py, trimmed.py)
gmsh/model/occ/addEllipseArc
¶Add an ellipse arc in the OpenCASCADE CAD representation, between the two points
startTag
and endTag
, and with center centerTag
and major
axis point majorTag
. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. Return the tag of the ellipse
arc. Note that OpenCASCADE does not allow creating ellipse arcs with the major
radius smaller than the minor radius.
gmsh/model/occ/addEllipse
¶Add an ellipse of center (x
, y
, z
) and radii r1
and
r2
along the x- and y-axes, respectively, in the OpenCASCADE CAD
representation. If tag
is positive, set the tag explicitly; otherwise a
new tag is selected automatically. If angle1
and angle2
are
specified, create an ellipse arc between the two angles. Return the tag of the
ellipse. Note that OpenCASCADE does not allow creating ellipses with the major
radius (along the x-axis) smaller than or equal to the minor radius (along the
y-axis): rotate the shape or use addCircle
in such cases.
gmsh/model/occ/addSpline
¶Add a spline (C2 b-spline) curve in the OpenCASCADE CAD representation, going
through the points pointTags
. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Create a periodic
curve if the first and last points are the same. Return the tag of the spline
curve.
gmsh/model/occ/addBSpline
¶Add a b-spline curve of degree degree
in the OpenCASCADE CAD
representation, with pointTags
control points. If weights
,
knots
or multiplicities
are not provided, default parameters are
computed automatically. If tag
is positive, set the tag explicitly;
otherwise a new tag is selected automatically. Create a periodic curve if the
first and last points are the same. Return the tag of the b-spline curve.
pointTags
, tag = -1
, degree = 3
, weights = []
, knots = []
, multiplicities = []
-
integer value
C++ (spline.cpp), Python (bspline_filling.py, spline.py)
gmsh/model/occ/addBezier
¶Add a Bezier curve in the OpenCASCADE CAD representation, with pointTags
control points. If tag
is positive, set the tag explicitly; otherwise a
new tag is selected automatically. Return the tag of the Bezier curve.
gmsh/model/occ/addWire
¶Add a wire (open or closed) in the OpenCASCADE CAD representation, formed by the
curves curveTags
. Note that an OpenCASCADE wire can be made of curves
that share geometrically identical (but topologically different) points. If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the wire.
curveTags
, tag = -1
, checkClosed = False
-
integer value
C++ (t19.cpp), Python (t19.py, bspline_bezier_trimmed.py, bspline_filling.py, pipe.py, trimmed.py)
gmsh/model/occ/addCurveLoop
¶Add a curve loop (a closed wire) in the OpenCASCADE CAD representation, formed
by the curves curveTags
. curveTags
should contain tags of curves
forming a closed loop. Note that an OpenCASCADE curve loop can be made of curves
that share geometrically identical (but topologically different) points. If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the curve loop.
gmsh/model/occ/addRectangle
¶Add a rectangle in the OpenCASCADE CAD representation, with lower left corner at
(x
, y
, z
) and upper right corner at (x
+ dx
,
y
+ dy
, z
). If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Round the corners if
roundedRadius
is nonzero. Return the tag of the rectangle.
x
, y
, z
, dx
, dy
, tag = -1
, roundedRadius = 0.
-
integer value
C++ (t17.cpp, t20.cpp, t21.cpp, adapt_mesh.cpp, edges.cpp, ...), Python (t17.py, t20.py, t21.py, adapt_mesh.py, crack3d.py, ...)
gmsh/model/occ/addDisk
¶Add a disk in the OpenCASCADE CAD representation, with center (xc
,
yc
, zc
) and radius rx
along the x-axis and ry
along
the y-axis. If tag
is positive, set the tag explicitly; otherwise a new
tag is selected automatically. Return the tag of the disk.
gmsh/model/occ/addPlaneSurface
¶Add a plane surface in the OpenCASCADE CAD representation, defined by one or
more curve loops (or closed wires) wireTags
. The first curve loop defines
the exterior contour; additional curve loop define holes. If tag
is
positive, set the tag explicitly; otherwise a new tag is selected automatically.
Return the tag of the surface.
gmsh/model/occ/addSurfaceFilling
¶Add a surface in the OpenCASCADE CAD representation, filling the curve loop
wireTag
. If tag
is positive, set the tag explicitly; otherwise a
new tag is selected automatically. Return the tag of the surface. If
pointTags
are provided, force the surface to pass through the given
points.
gmsh/model/occ/addBSplineFilling
¶Add a BSpline surface in the OpenCASCADE CAD representation, filling the curve
loop wireTag
. The curve loop should be made of 2, 3 or 4 BSpline curves.
The optional type
argument specifies the type of filling: "Stretch"
creates the flattest patch, "Curved" (the default) creates the most rounded
patch, and "Coons" creates a rounded patch with less depth than "Curved". If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the surface.
wireTag
, tag = -1
, type = ""
-
integer value
Python (bspline_filling.py)
gmsh/model/occ/addBezierFilling
¶Add a Bezier surface in the OpenCASCADE CAD representation, filling the curve
loop wireTag
. The curve loop should be made of 2, 3 or 4 Bezier curves.
The optional type
argument specifies the type of filling: "Stretch"
creates the flattest patch, "Curved" (the default) creates the most rounded
patch, and "Coons" creates a rounded patch with less depth than "Curved". If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the surface.
gmsh/model/occ/addBSplineSurface
¶Add a b-spline surface of degree degreeU
x degreeV
in the
OpenCASCADE CAD representation, with pointTags
control points given as a
single vector [Pu1v1, ... PunumPointsU
v1, Pu1v2, ...]. If weights
,
knotsU
, knotsV
, multiplicitiesU
or multiplicitiesV
are not provided, default parameters are computed automatically. If tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. If wireTags
is provided, trim the b-spline patch using the
provided wires: the first wire defines the external contour, the others define
holes. If wire3D
is set, consider wire curves as 3D curves and project
them on the b-spline surface; otherwise consider the wire curves as defined in
the parametric space of the surface. Return the tag of the b-spline surface.
pointTags
, numPointsU
, tag = -1
, degreeU = 3
, degreeV = 3
, weights = []
, knotsU = []
, knotsV = []
, multiplicitiesU = []
, multiplicitiesV = []
, wireTags = []
, wire3D = False
-
integer value
Python (bspline_bezier_patches.py, bspline_bezier_trimmed.py, terrain_bspline.py)
gmsh/model/occ/addBezierSurface
¶Add a Bezier surface in the OpenCASCADE CAD representation, with
pointTags
control points given as a single vector [Pu1v1, ...
PunumPointsU
v1, Pu1v2, ...]. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. If wireTags
is
provided, trim the Bezier patch using the provided wires: the first wire defines
the external contour, the others define holes. If wire3D
is set, consider
wire curves as 3D curves and project them on the Bezier surface; otherwise
consider the wire curves as defined in the parametric space of the surface.
Return the tag of the Bezier surface.
pointTags
, numPointsU
, tag = -1
, wireTags = []
, wire3D = False
-
integer value
Python (bspline_bezier_patches.py)
gmsh/model/occ/addTrimmedSurface
¶Trim the surface surfaceTag
with the wires wireTags
, replacing any
existing trimming curves. The first wire defines the external contour, the
others define holes. If wire3D
is set, consider wire curves as 3D curves
and project them on the surface; otherwise consider the wire curves as defined
in the parametric space of the surface. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Return the tag of the
trimmed surface.
surfaceTag
, wireTags = []
, wire3D = False
, tag = -1
-
integer value
Python (trimmed.py)
gmsh/model/occ/addSurfaceLoop
¶Add a surface loop (a closed shell) in the OpenCASCADE CAD representation,
formed by surfaceTags
. If tag
is positive, set the tag
explicitly; otherwise a new tag is selected automatically. Return the tag of the
surface loop. Setting sewing
allows to build a shell made of surfaces
that share geometrically identical (but topologically different) curves.
gmsh/model/occ/addVolume
¶Add a volume (a region) in the OpenCASCADE CAD representation, defined by one or
more surface loops shellTags
. The first surface loop defines the exterior
boundary; additional surface loop define holes. If tag
is positive, set
the tag explicitly; otherwise a new tag is selected automatically. Return the
tag of the volume.
gmsh/model/occ/addSphere
¶Add a sphere of center (xc
, yc
, zc
) and radius r
in
the OpenCASCADE CAD representation. The optional angle1
and angle2
arguments define the polar angle opening (from -Pi/2 to Pi/2). The optional
angle3
argument defines the azimuthal opening (from 0 to 2*Pi). If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. Return the tag of the sphere.
xc
, yc
, zc
, radius
, tag = -1
, angle1 = -pi/2
, angle2 = pi/2
, angle3 = 2*pi
-
integer value
C++ (t16.cpp, t18.cpp, boolean.cpp, faces.cpp, gui.cpp), Python (t16.py, t18.py, boolean2.py, boolean.py, gui.py, ...)
gmsh/model/occ/addBox
¶Add a parallelepipedic box in the OpenCASCADE CAD representation, defined by a
point (x
, y
, z
) and the extents along the x-, y- and
z-axes. If tag
is positive, set the tag explicitly; otherwise a new tag
is selected automatically. Return the tag of the box.
x
, y
, z
, dx
, dy
, dz
, tag = -1
-
integer value
C++ (t16.cpp, t18.cpp, x4.cpp, boolean.cpp, faces.cpp, ...), Python (t16.py, t18.py, x4.py, boolean2.py, boolean.py, ...)
gmsh/model/occ/addCylinder
¶Add a cylinder in the OpenCASCADE CAD representation, defined by the center
(x
, y
, z
) of its first circular face, the 3 components
(dx
, dy
, dz
) of the vector defining its axis and its radius
r
. The optional angle
argument defines the angular opening (from 0
to 2*Pi). If tag
is positive, set the tag explicitly; otherwise a new tag
is selected automatically. Return the tag of the cylinder.
x
, y
, z
, dx
, dy
, dz
, r
, tag = -1
, angle = 2*pi
-
integer value
C++ (boolean.cpp, gui.cpp), Python (boolean2.py, boolean.py, gui.py)
gmsh/model/occ/addCone
¶Add a cone in the OpenCASCADE CAD representation, defined by the center
(x
, y
, z
) of its first circular face, the 3 components of
the vector (dx
, dy
, dz
) defining its axis and the two radii
r1
and r2
of the faces (these radii can be zero). If tag
is
positive, set the tag explicitly; otherwise a new tag is selected automatically.
angle
defines the optional angular opening (from 0 to 2*Pi). Return the
tag of the cone.
gmsh/model/occ/addWedge
¶Add a right angular wedge in the OpenCASCADE CAD representation, defined by the
right-angle point (x
, y
, z
) and the 3 extends along the x-,
y- and z-axes (dx
, dy
, dz
). If tag
is positive, set
the tag explicitly; otherwise a new tag is selected automatically. The optional
argument ltx
defines the top extent along the x-axis. Return the tag of
the wedge.
gmsh/model/occ/addTorus
¶Add a torus in the OpenCASCADE CAD representation, defined by its center
(x
, y
, z
) and its 2 radii r
and r2
. If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically. The optional argument angle
defines the angular opening
(from 0 to 2*Pi). Return the tag of the wedge.
gmsh/model/occ/addThruSections
¶Add a volume (if the optional argument makeSolid
is set) or surfaces in
the OpenCASCADE CAD representation, defined through the open or closed wires
wireTags
. If tag
is positive, set the tag explicitly; otherwise a
new tag is selected automatically. The new entities are returned in
outDimTags
. If the optional argument makeRuled
is set, the
surfaces created on the boundary are forced to be ruled surfaces. If
maxDegree
is positive, set the maximal degree of resulting surface.
gmsh/model/occ/addThickSolid
¶Add a hollowed volume in the OpenCASCADE CAD representation, built from an
initial volume volumeTag
and a set of faces from this volume
excludeSurfaceTags
, which are to be removed. The remaining faces of the
volume become the walls of the hollowed solid, with thickness offset
. If
tag
is positive, set the tag explicitly; otherwise a new tag is selected
automatically.
gmsh/model/occ/extrude
¶Extrude the entities dimTags
in the OpenCASCADE CAD representation, using
a translation along (dx
, dy
, dz
). Return extruded entities
in outDimTags
. If numElements
is not empty, also extrude the mesh:
the entries in numElements
give the number of elements in each layer. If
height
is not empty, it provides the (cumulative) height of the different
layers, normalized to 1. If recombine
is set, recombine the mesh in the
layers.
gmsh/model/occ/revolve
¶Extrude the entities dimTags
in the OpenCASCADE CAD representation, using
a rotation of angle
radians around the axis of revolution defined by the
point (x
, y
, z
) and the direction (ax
, ay
,
az
). Return extruded entities in outDimTags
. If numElements
is not empty, also extrude the mesh: the entries in numElements
give the
number of elements in each layer. If height
is not empty, it provides the
(cumulative) height of the different layers, normalized to 1. When the mesh is
extruded the angle should be strictly smaller than 2*Pi. If recombine
is
set, recombine the mesh in the layers.
gmsh/model/occ/addPipe
¶Add a pipe in the OpenCASCADE CAD representation, by extruding the entities
dimTags
along the wire wireTag
. The type of sweep can be specified
with trihedron
(possible values: "DiscreteTrihedron", "CorrectedFrenet",
"Fixed", "Frenet", "ConstantNormal", "Darboux", "GuideAC", "GuidePlan",
"GuideACWithContact", "GuidePlanWithContact"). If trihedron
is not
provided, "DiscreteTrihedron" is assumed. Return the pipe in outDimTags
.
gmsh/model/occ/fillet
¶Fillet the volumes volumeTags
on the curves curveTags
with radii
radii
. The radii
vector can either contain a single radius, as
many radii as curveTags
, or twice as many as curveTags
(in which
case different radii are provided for the begin and end points of the curves).
Return the filleted entities in outDimTags
. Remove the original volume if
removeVolume
is set.
gmsh/model/occ/chamfer
¶Chamfer the volumes volumeTags
on the curves curveTags
with
distances distances
measured on surfaces surfaceTags
. The
distances
vector can either contain a single distance, as many distances
as curveTags
and surfaceTags
, or twice as many as curveTags
and surfaceTags
(in which case the first in each pair is measured on the
corresponding surface in surfaceTags
, the other on the other adjacent
surface). Return the chamfered entities in outDimTags
. Remove the
original volume if removeVolume
is set.
gmsh/model/occ/fuse
¶Compute the boolean union (the fusion) of the entities objectDimTags
and
toolDimTags
in the OpenCASCADE CAD representation. Return the resulting
entities in outDimTags
. If tag
is positive, try to set the tag
explicitly (only valid if the boolean operation results in a single entity).
Remove the object if removeObject
is set. Remove the tool if
removeTool
is set.
objectDimTags
, toolDimTags
, tag = -1
, removeObject = True
, removeTool = True
outDimTags
, outDimTagsMap
-
C++ (boolean.cpp, gui.cpp), Python (boolean2.py, boolean.py, gui.py)
gmsh/model/occ/intersect
¶Compute the boolean intersection (the common parts) of the entities
objectDimTags
and toolDimTags
in the OpenCASCADE CAD
representation. Return the resulting entities in outDimTags
. If
tag
is positive, try to set the tag explicitly (only valid if the boolean
operation results in a single entity). Remove the object if removeObject
is set. Remove the tool if removeTool
is set.
objectDimTags
, toolDimTags
, tag = -1
, removeObject = True
, removeTool = True
outDimTags
, outDimTagsMap
-
C++ (boolean.cpp, gui.cpp), Python (boolean2.py, boolean.py, gui.py)
gmsh/model/occ/cut
¶Compute the boolean difference between the entities objectDimTags
and
toolDimTags
in the OpenCASCADE CAD representation. Return the resulting
entities in outDimTags
. If tag
is positive, try to set the tag
explicitly (only valid if the boolean operation results in a single entity).
Remove the object if removeObject
is set. Remove the tool if
removeTool
is set.
objectDimTags
, toolDimTags
, tag = -1
, removeObject = True
, removeTool = True
outDimTags
, outDimTagsMap
-
C++ (t16.cpp, boolean.cpp, gui.cpp), Python (t16.py, boolean2.py, boolean.py, gui.py, spherical_surf.py)
gmsh/model/occ/fragment
¶Compute the boolean fragments (general fuse) resulting from the intersection of
the entities objectDimTags
and toolDimTags
in the OpenCASCADE CAD
representation, making all iterfaces conformal. When applied to entities of
different dimensions, the lower dimensional entities will be automatically
embedded in the higher dimensional entities if they are not on their boundary.
Return the resulting entities in outDimTags
. If tag
is positive,
try to set the tag explicitly (only valid if the boolean operation results in a
single entity). Remove the object if removeObject
is set. Remove the tool
if removeTool
is set.
gmsh/model/occ/translate
¶Translate the entities dimTags
in the OpenCASCADE CAD representation
along (dx
, dy
, dz
).
gmsh/model/occ/rotate
¶Rotate the entities dimTags
in the OpenCASCADE CAD representation by
angle
radians around the axis of revolution defined by the point
(x
, y
, z
) and the direction (ax
, ay
,
az
).
gmsh/model/occ/dilate
¶Scale the entities dimTags
in the OpenCASCADE CAD representation by
factors a
, b
and c
along the three coordinate axes; use
(x
, y
, z
) as the center of the homothetic transformation.
gmsh/model/occ/mirror
¶Mirror the entities dimTags
in the OpenCASCADE CAD representation, with
respect to the plane of equation a
* x + b
* y + c
* z +
d
= 0.
gmsh/model/occ/symmetrize
¶Mirror the entities dimTags
in the OpenCASCADE CAD representation, with
respect to the plane of equation a
* x + b
* y + c
* z +
d
= 0. (This is a synonym for mirror
, which will be deprecated in
a future release.)
gmsh/model/occ/affineTransform
¶Apply a general affine transformation matrix a
(16 entries of a 4x4
matrix, by row; only the 12 first can be provided for convenience) to the
entities dimTags
in the OpenCASCADE CAD representation.
gmsh/model/occ/copy
¶Copy the entities dimTags
in the OpenCASCADE CAD representation; the new
entities are returned in outDimTags
.
gmsh/model/occ/remove
¶Remove the entities dimTags
in the OpenCASCADE CAD representation. If
recursive
is true, remove all the entities on their boundaries, down to
dimension 0.
gmsh/model/occ/removeAllDuplicates
¶Remove all duplicate entities in the OpenCASCADE CAD representation (different entities at the same geometrical location) after intersecting (using boolean fragments) all highest dimensional entities.
-
-
-
Python (bspline_bezier_patches.py)
gmsh/model/occ/healShapes
¶Apply various healing procedures to the entities dimTags
(or to all the
entities in the model if dimTags
is empty) in the OpenCASCADE CAD
representation. Return the healed entities in outDimTags
. Available
healing options are listed in the Gmsh reference manual.
gmsh/model/occ/importShapes
¶Import BREP, STEP or IGES shapes from the file fileName
in the
OpenCASCADE CAD representation. The imported entities are returned in
outDimTags
. If the optional argument highestDimOnly
is set, only
import the highest dimensional entities in the file. The optional argument
format
can be used to force the format of the file (currently "brep",
"step" or "iges").
gmsh/model/occ/importShapesNativePointer
¶Imports an OpenCASCADE shape
by providing a pointer to a native
OpenCASCADE TopoDS_Shape
object (passed as a pointer to void). The
imported entities are returned in outDimTags
. If the optional argument
highestDimOnly
is set, only import the highest dimensional entities in
shape
. For C and C++ only. Warning: this function is unsafe, as providing
an invalid pointer will lead to undefined behavior.
gmsh/model/occ/getEntities
¶Get all the OpenCASCADE entities. If dim
is >= 0, return only the
entities of the specified dimension (e.g. points if dim
== 0). The
entities are returned as a vector of (dim, tag) integer pairs.
gmsh/model/occ/getEntitiesInBoundingBox
¶Get the OpenCASCADE entities in the bounding box defined by the two points
(xmin
, ymin
, zmin
) and (xmax
, ymax
,
zmax
). If dim
is >= 0, return only the entities of the specified
dimension (e.g. points if dim
== 0).
gmsh/model/occ/getBoundingBox
¶Get the bounding box (xmin
, ymin
, zmin
), (xmax
,
ymax
, zmax
) of the OpenCASCADE entity of dimension dim
and
tag tag
.
gmsh/model/occ/getMass
¶Get the mass of the OpenCASCADE entity of dimension dim
and tag
tag
.
gmsh/model/occ/getCenterOfMass
¶Get the center of mass of the OpenCASCADE entity of dimension dim
and tag
tag
.
gmsh/model/occ/getMatrixOfInertia
¶Get the matrix of inertia (by row) of the OpenCASCADE entity of dimension
dim
and tag tag
.
gmsh/model/occ/getMaxTag
¶Get the maximum tag of entities of dimension dim
in the OpenCASCADE CAD
representation.
gmsh/model/occ/setMaxTag
¶Set the maximum tag maxTag
for entities of dimension dim
in the
OpenCASCADE CAD representation.
gmsh/model/occ/synchronize
¶Synchronize the OpenCASCADE CAD representation with the current Gmsh model. This can be called at any time, but since it involves a non trivial amount of processing, the number of synchronization points should normally be minimized. Without synchronization the entities in the OpenCASCADE CAD representation are not available to any function outside of the OpenCASCADE CAD kernel functions.
Next: Namespace gmsh/view
: post-processing view functions, Previous: Namespace gmsh/model/occ
: OpenCASCADE CAD kernel functions, Up: Gmsh API [Contents][Index]
gmsh/model/occ/mesh
: OpenCASCADE CAD kernel meshing constraintsgmsh/model/occ/mesh/setSize
¶Set a mesh size constraint on the entities dimTags
in the OpenCASCADE CAD
representation. Currently only entities of dimension 0 (points) are handled.
Next: Namespace gmsh/plugin
: plugin functions, Previous: Namespace gmsh/model/occ/mesh
: OpenCASCADE CAD kernel meshing constraints, Up: Gmsh API [Contents][Index]
gmsh/view
: post-processing view functionsgmsh/view/add
¶Add a new post-processing view, with name name
. If tag
is positive
use it (and remove the view with that tag if it already exists), otherwise
associate a new tag. Return the view tag.
name
, tag = -1
-
integer value
C++ (t4.cpp, x3.cpp, x4.cpp, adapt_mesh.cpp, plugin.cpp, ...), Python (t4.py, x3.py, x4.py, adapt_mesh.py, copy_mesh.py, ...)
gmsh/view/remove
¶Remove the view with tag tag
.
gmsh/view/getIndex
¶Get the index of the view with tag tag
in the list of currently loaded
views. This dynamic index (it can change when views are removed) is used to
access view options.
gmsh/view/getTags
¶Get the tags of all views.
gmsh/view/addModelData
¶Add model-based post-processing data to the view with tag tag
.
modelName
identifies the model the data is attached to. dataType
specifies the type of data, currently either "NodeData", "ElementData" or
"ElementNodeData". step
specifies the identifier (>= 0) of the data in a
sequence. tags
gives the tags of the nodes or elements in the mesh to
which the data is associated. data
is a vector of the same length as
tags
: each entry is the vector of double precision numbers representing
the data associated with the corresponding tag. The optional time
argument associate a time value with the data. numComponents
gives the
number of data components (1 for scalar data, 3 for vector data, etc.) per
entity; if negative, it is automatically inferred (when possible) from the input
data. partition
allows to specify data in several sub-sets.
tag
, step
, modelName
, dataType
, tags
, data
, time = 0.
, numComponents = -1
, partition = 0
-
-
C++ (adapt_mesh.cpp, plugin.cpp, view.cpp), Python (adapt_mesh.py, plugin.py, poisson.py, view.py)
gmsh/view/addHomogeneousModelData
¶Add homogeneous model-based post-processing data to the view with tag
tag
. The arguments have the same meaning as in addModelData
,
except that data
is supposed to be homogeneous and is thus flattened in a
single vector. For data types that can lead to different data sizes per tag
(like "ElementNodeData"), the data should be padded.
gmsh/view/getModelData
¶Get model-based post-processing data from the view with tag tag
at step
step
. Return the data
associated to the nodes or the elements with
tags tags
, as well as the dataType
and the number of components
numComponents
.
tag
, step
dataType
, tags
, data
, time
, numComponents
-
C++ (get_data_perf.cpp, plugin.cpp), Python (get_data_perf.py, mesh_quality.py, plugin.py)
gmsh/view/getHomogeneousModelData
¶Get homogeneous model-based post-processing data from the view with tag
tag
at step step
. The arguments have the same meaning as in
getModelData
, except that data
is returned flattened in a single
vector, with the appropriate padding if necessary.
tag
, step
dataType
, tags
, data
, time
, numComponents
-
C++ (get_data_perf.cpp), Python (get_data_perf.py)
gmsh/view/addListData
¶Add list-based post-processing data to the view with tag tag
. List-based
datasets are independent from any model and any mesh. dataType
identifies
the data by concatenating the field type ("S" for scalar, "V" for vector, "T"
for tensor) and the element type ("P" for point, "L" for line, "T" for triangle,
"S" for tetrahedron, "I" for prism, "H" for hexaHedron, "Y" for pyramid). For
example dataType
should be "ST" for a scalar field on triangles.
numEle
gives the number of elements in the data. data
contains the
data for the numEle
elements, concatenated, with node coordinates
followed by values per node, repeated for each step: [e1x1, ..., e1xn, e1y1,
..., e1yn, e1z1, ..., e1zn, e1v1..., e1vN, e2x1, ...].
tag
, dataType
, numEle
, data
-
-
C++ (x3.cpp, viewlist.cpp), Python (x3.py, normals.py, view_combine.py, viewlist.py)
gmsh/view/getListData
¶Get list-based post-processing data from the view with tag tag
. Return
the types dataTypes
, the number of elements numElements
for each
data type and the data
for each data type.
gmsh/view/addListDataString
¶Add a string to a list-based post-processing view with tag tag
. If
coord
contains 3 coordinates the string is positioned in the 3D model
space ("3D string"); if it contains 2 coordinates it is positioned in the 2D
graphics viewport ("2D string"). data
contains one or more (for multistep
views) strings. style
contains key-value pairs of styling parameters,
concatenated. Available keys are "Font" (possible values: "Times-Roman", "Times-
Bold", "Times-Italic", "Times-BoldItalic", "Helvetica", "Helvetica-Bold",
"Helvetica-Oblique", "Helvetica-BoldOblique", "Courier", "Courier-Bold",
"Courier-Oblique", "Courier-BoldOblique", "Symbol", "ZapfDingbats", "Screen"),
"FontSize" and "Align" (possible values: "Left" or "BottomLeft", "Center" or
"BottomCenter", "Right" or "BottomRight", "TopLeft", "TopCenter", "TopRight",
"CenterLeft", "CenterCenter", "CenterRight").
gmsh/view/getListDataStrings
¶Get list-based post-processing data strings (2D strings if dim
= 2, 3D
strings if dim
= 3) from the view with tag tag
. Return the
coordinates in coord
, the strings in data
and the styles in
style
.
gmsh/view/setInterpolationMatrices
¶Set interpolation matrices for the element family type
("Line",
"Triangle", "Quadrangle", "Tetrahedron", "Hexahedron", "Prism", "Pyramid") in
the view tag
. The approximation of the values over an element is written
as a linear combination of d
basis functions f_i(u, v, w) = sum_(j = 0,
..., d
- 1) coef
[i][j] u^exp
[j][0] v^exp
[j][1]
w^exp
[j][2], i = 0, ..., d
-1, with u, v, w the coordinates in the
reference element. The coef
matrix (of size d
x d
) and the
exp
matrix (of size d
x 3) are stored as vectors, by row. If
dGeo
is positive, use coefGeo
and expGeo
to define the
interpolation of the x, y, z coordinates of the element in terms of the u, v, w
coordinates, in exactly the same way. If d
< 0, remove the interpolation
matrices.
gmsh/view/addAlias
¶Add a post-processing view as an alias
of the reference view with tag
refTag
. If copyOptions
is set, copy the options of the reference
view. If tag
is positive use it (and remove the view with that tag if it
already exists), otherwise associate a new tag. Return the view tag.
refTag
, copyOptions = False
, tag = -1
-
integer value
Python (view_combine.py)
gmsh/view/copyOptions
¶Copy the options from the view with tag refTag
to the view with tag
tag
.
gmsh/view/combine
¶Combine elements (if what
== "elements") or steps (if what
==
"steps") of all views (how
== "all"), all visible views (how
==
"visible") or all views having the same name (how
== "name"). Remove
original views if remove
is set.
what
, how
, remove = True
, copyOptions = True
-
-
Python (view_combine.py)
gmsh/view/probe
¶Probe the view tag
for its value
at point (x
, y
,
z
). Return only the value at step step
is step
is positive.
Return only values with numComp
if numComp
is positive. Return the
gradient of the value
if gradient
is set. Probes with a
geometrical tolerance (in the reference unit cube) of tolerance
if
tolerance
is not zero. Return the result from the element described by
its coordinates if xElementCoord
, yElementCoord
and
zElementCoord
are provided. If dim
is >= 0, return only elements
of the specified dimension.
gmsh/view/write
¶Write the view to a file fileName
. The export format is determined by the
file extension. Append to the file if append
is set.
tag
, fileName
, append = False
-
-
C++ (x3.cpp, x4.cpp, adapt_mesh.cpp, plugin.cpp, view.cpp, ...), Python (x3.py, x4.py, adapt_mesh.py, normals.py, plugin.py, ...)
gmsh/view/setVisibilityPerWindow
¶Set the global visibility of the view tag
per window to value
,
where windowIndex
identifies the window in the window list.
Next: Namespace gmsh/graphics
: graphics functions, Previous: Namespace gmsh/view
: post-processing view functions, Up: Gmsh API [Contents][Index]
gmsh/plugin
: plugin functionsgmsh/plugin/setNumber
¶Set the numerical option option
to the value value
for plugin
name
.
name
, option
, value
-
-
C++ (t9.cpp, t21.cpp, get_data_perf.cpp, partition.cpp, plugin.cpp), Python (t9.py, t21.py, crack3d.py, crack.py, get_data_perf.py, ...)
gmsh/plugin/setString
¶Set the string option option
to the value value
for plugin
name
.
gmsh/plugin/run
¶Run the plugin name
.
name
-
-
C++ (t9.cpp, t21.cpp, get_data_perf.cpp, partition.cpp, plugin.cpp), Python (t9.py, t21.py, crack3d.py, crack.py, get_data_perf.py, ...)
Next: Namespace gmsh/fltk
: FLTK graphical user interface functions, Previous: Namespace gmsh/plugin
: plugin functions, Up: Gmsh API [Contents][Index]
gmsh/graphics
: graphics functionsgmsh/graphics/draw
¶Draw all the OpenGL scenes.
Next: Namespace gmsh/onelab
: ONELAB server functions, Previous: Namespace gmsh/graphics
: graphics functions, Up: Gmsh API [Contents][Index]
gmsh/fltk
: FLTK graphical user interface functionsgmsh/fltk/initialize
¶Create the FLTK graphical user interface. Can only be called in the main thread.
gmsh/fltk/wait
¶Wait at most time
seconds for user interface events and return. If
time
< 0, wait indefinitely. First automatically create the user
interface if it has not yet been initialized. Can only be called in the main
thread.
gmsh/fltk/update
¶Update the user interface (potentially creating new widgets and windows). First
automatically create the user interface if it has not yet been initialized. Can
only be called in the main thread: use awake("update")
to trigger an
update of the user interface from another thread.
-
-
-
C++ (custom_gui.cpp), Python (custom_gui.py, prepro.py)
gmsh/fltk/awake
¶Awake the main user interface thread and process pending events, and optionally
perform an action (currently the only action
allowed is "update").
action = ""
-
-
C++ (custom_gui.cpp), Python (custom_gui.py)
gmsh/fltk/lock
¶Block the current thread until it can safely modify the user interface.
-
-
-
C++ (custom_gui.cpp), Python (custom_gui.py)
gmsh/fltk/unlock
¶Release the lock that was set using lock.
-
-
-
C++ (custom_gui.cpp), Python (custom_gui.py)
gmsh/fltk/run
¶Run the event loop of the graphical user interface, i.e. repeatedly call
wait()
. First automatically create the user interface if it has not yet
been initialized. Can only be called in the main thread.
gmsh/fltk/isAvailable
¶Check if the user interface is available (e.g. to detect if it has been closed).
gmsh/fltk/selectEntities
¶Select entities in the user interface. If dim
is >= 0, return only the
entities of the specified dimension (e.g. points if dim
== 0).
gmsh/fltk/selectElements
¶Select elements in the user interface.
gmsh/fltk/selectViews
¶Select views in the user interface.
gmsh/fltk/splitCurrentWindow
¶Split the current window horizontally (if how
= "h") or vertically (if
how
= "v"), using ratio ratio
. If how
= "u", restore a
single window.
how = "v"
, ratio = 0.5
-
-
Python (split_window.py)
gmsh/fltk/setCurrentWindow
¶Set the current window by speficying its index (starting at 0) in the list of all windows. When new windows are created by splits, new windows are appended at the end of the list.
windowIndex = 0
-
-
Python (split_window.py)
gmsh/fltk/setStatusMessage
¶Set a status message in the current window. If graphics
is set, display
the message inside the graphic window instead of the status bar.
gmsh/fltk/showContextWindow
¶Show context window for the entity of dimension dim
and tag tag
.
gmsh/fltk/openTreeItem
¶Open the name
item in the menu tree.
gmsh/fltk/closeTreeItem
¶Close the name
item in the menu tree.
Next: Namespace gmsh/logger
: information logging functions, Previous: Namespace gmsh/fltk
: FLTK graphical user interface functions, Up: Gmsh API [Contents][Index]
gmsh/onelab
: ONELAB server functionsgmsh/onelab/set
¶Set one or more parameters in the ONELAB database, encoded in format
.
data
, format = "json"
-
-
C++ (t3.cpp, t13.cpp, t21.cpp, custom_gui.cpp), Python (t3.py, t13.py, t21.py, custom_gui.py, onelab_test.py, ...)
gmsh/onelab/get
¶Get all the parameters (or a single one if name
is specified) from the
ONELAB database, encoded in format
.
name = ""
, format = "json"
data
-
C++ (onelab_data.cpp), Python (onelab_data.py, onelab_test.py, prepro.py)
gmsh/onelab/getNames
¶Get the names of the parameters in the ONELAB database matching the
search
regular expression. If search
is empty, return all the
names.
gmsh/onelab/setNumber
¶Set the value of the number parameter name
in the ONELAB database. Create
the parameter if it does not exist; update the value if the parameter exists.
name
, value
-
-
C++ (custom_gui.cpp), Python (custom_gui.py, onelab_test.py)
gmsh/onelab/setString
¶Set the value of the string parameter name
in the ONELAB database. Create
the parameter if it does not exist; update the value if the parameter exists.
name
, value
-
-
C++ (t3.cpp, t13.cpp, t21.cpp, custom_gui.cpp), Python (t3.py, t13.py, t21.py, custom_gui.py, onelab_test.py, ...)
gmsh/onelab/getNumber
¶Get the value of the number parameter name
from the ONELAB database.
Return an empty vector if the parameter does not exist.
gmsh/onelab/getString
¶Get the value of the string parameter name
from the ONELAB database.
Return an empty vector if the parameter does not exist.
gmsh/onelab/clear
¶Clear the ONELAB database, or remove a single parameter if name
is given.
name = ""
-
-
Python (onelab_test.py)
gmsh/onelab/run
¶Run a ONELAB client. If name
is provided, create a new ONELAB client with
name name
and executes command
. If not, try to run a client that
might be linked to the processed input files.
name = ""
, command = ""
-
-
C++ (onelab_data.cpp), Python (onelab_data.py)
Previous: Namespace gmsh/onelab
: ONELAB server functions, Up: Gmsh API [Contents][Index]
gmsh/logger
: information logging functionsgmsh/logger/write
¶Write a message
. level
can be "info", "warning" or "error".
gmsh/logger/start
¶Start logging messages.
gmsh/logger/get
¶Get logged messages.
gmsh/logger/stop
¶Stop logging messages.
gmsh/logger/getWallTime
¶Return wall clock time.
-
-
floating point value
C++ (custom_gui.cpp, import_perf.cpp), Python (import_perf.py)
gmsh/logger/getCpuTime
¶Return CPU time.
gmsh/logger/getLastError
¶Return last error message, if any.
Next: Frequently asked questions, Previous: Gmsh API, Up: Gmsh [Contents][Index]
Gmsh is written in C++, the scripting language is parsed using Lex and Yacc (actually, Flex and Bison), and the GUI relies on OpenGL for the 3D graphics and FLTK (http://www.fltk.org) for the widgets (menus, buttons, etc.). Gmsh’s build system is based on CMake (http://www.cmake.org). Practical notes on how to compile Gmsh’s source code are provided in Compiling the source code (see also Frequently asked questions).
This section is for developers who would like to contribute directly to the Gmsh source code. Gmsh’s official Git repository is located at https://gitlab.onelab.info/gmsh/gmsh. The wiki (https://gitlab.onelab.info/gmsh/gmsh/wikis/Git-cheat-sheet) contains instructions on how to create feature branches and submit merge requests.
Next: Coding style, Previous: Information for developers, Up: Information for developers [Contents][Index]
Gmsh’s code is structured in several subdirectories, roughly separated between the four core modules (Geo, Mesh, Solver, Post) and associated utilities (Common, Numeric) on one hand, and the graphics (Graphics) and interface (Fltk, Parser, api) code on the other.
The geometry module is based on a model class (Geo/GModel.h), and abstract entity classes for geometrical points (Geo/GVertex.h), curves (Geo/GEdge.h), surfaces (Geo/GFace.h) and volumes (Geo/GRegion.h). Concrete implementations of these classes are provided for each supported CAD kernel (e.g. Geo/gmshVertex.h for points in Gmsh’s built-in CAD kernel, or Geo/OCCVertex.h for points from OpenCASCADE). All these elementary model entities derive from Geo/GEntity.h. Physical groups are simply stored as integer tags in the entities.
A mesh is composed of elements: mesh points (Geo/MPoint.h), lines (Geo/MLine.h), triangles (Geo/MTriangle.h), quadrangles (Geo/MQuadrangle.h), tetrahedra (Geo/MTetrahedron.h), etc. All the mesh elements are derived from Geo/MElement.h, and are stored in the corresponding model entities: one mesh point per geometrical point, mesh lines in geometrical curves, triangles and quadrangles in surfaces, etc. The elements are defined in terms of their nodes (Geo/MVertex.h). Each model entity stores only its internal nodes: nodes on boundaries or on embedded entities are stored in the associated bounding/embedded entity.
The post-processing module is based on the concept of views (Post/PView.h) and abstract data containers (derived from Post/PViewData.h). Data can be either mesh-based (Post/PViewDataGModel.h), in which case the view is linked to one or more models, or list-based (Post/PViewDataLis.h), in which case all the relevant geometrical information is self-contained in the view.
Next: Adding a new option, Previous: Source code structure, Up: Information for developers [Contents][Index]
If you plan to contribute code to the Gmsh project, here are some easy rules to make the code easy to read/debug/maintain:
clang-format
tool to apply these rules automatically (the rules
are defined in the
.clang-format
file.)
Msg::
class to print information or errors
valgrind --leak-check=full gmsh file.geo -3
.
Previous: Coding style, Up: Information for developers [Contents][Index]
To add a new option in Gmsh:
CTX
class
(Common/Context.h
if it’s a classical option, or in the PViewOptions
class
(Post/PViewOptions.h)
if it’s a post-processing view-dependent option;
opt_XXX
) and a default value for this
option;
opt_XXX
in
Common/Options.cpp
(and add the prototype in
Common/Options.h);
Next: Version history, Previous: Information for developers, Up: Gmsh [Contents][Index]
Next: Installation problems, Previous: Frequently asked questions, Up: Frequently asked questions [Contents][Index]
Gmsh is an automatic three-dimensional finite element mesh generator with built-in pre- and post-processing facilities. With Gmsh you can create or import 1D, 2D and 3D geometrical models, mesh them, launch external finite element solvers and visualize solutions. Gmsh can be used either as a stand-alone program (graphical or not) or as a library to integrate in C++, C, Python or Julia codes.
Gmsh is distributed under the terms of the GNU General Public License, with an exception to allow for easier linking with external libraries. See License for more information.
Nothing... The name was derived from a previous version called “msh” (a shortcut for “mesh”), with the “g” prefix added to differentiate it. The default mesh file format used by Gmsh still uses the .msh extension.
In English people tend to pronounce ‘Gmsh’ as “gee-mesh”.
Yes, using the Gmsh API (see Gmsh API). See Copying conditions for the licensing constraints.
https://gmsh.info is the primary location to obtain information about Gmsh. There you will for example find the complete reference manual and the bug tracking database.
Next: General questions, Previous: The basics, Up: Frequently asked questions [Contents][Index]
Gmsh runs on Windows, Mac OS X, Linux and most Unix variants. Gmsh is also available as part of the ONELAB package on Android and iOS tablets and phones.
You should have the OpenGL libraries installed on your system, and in the path of the library loader. A free replacement for OpenGL can be found at http://www.mesa3d.org.
You need cmake (http://www.cmake.org) and a C++ compiler. See Compiling the source code for more information.
Gmsh will attempt to save temporary files and persistent configuration
options first in the $GMSH_HOME
directory, then in
$APPDATA
(on Windows) or $HOME
(on other OSes), then in
$TMP
, and finally in $TEMP
, in that order. If none of
these variables are defined, Gmsh will try to save/load its
configuration files from the current working directory.
Next: Geometry module, Previous: Installation problems, Up: Frequently asked questions [Contents][Index]
On Windows, if your system complains about missing OPENGL32.DLL or GLU32.DLL libraries, then OpenGL is not properly installed on your machine. You can download OpenGL from Microsoft’s web site, or directly from http://www.opengl.org.
On Unix try ‘ldd gmsh’ (or ‘otool -L gmsh’ on Mac OS X) to check if all the required shared libraries are installed on your system. If not, install them. If it still doesn’t work, recompile Gmsh from the source code.
Disable opaque move in your window manager.
Are you are executing Gmsh from a remote host (via the network) without GLX? You should turn double buffering off (with the ‘-nodb’ command line option).
No, there isn’t. This “ghost triangulation” is due to the fact that most PostScript previewers nowadays antialias the graphic primitives when they display the page on screen. (For example, in gv, you can disable antialising with the ‘State->Antialias’ menu.) You should not see this ghost triangulation in the printed output (on paper).
Just choose the appropriate format in ‘File->Export’. By default Gmsh guesses the format from the file extension, so you can just type myfile.jpg in the dialog and Gmsh will automatically create a JPEG image file.
You can specify the dimension in the dialog (e.g. set the width of the
image to 5000 pixels; leaving one dimension negative will rescale using
the natural aspect ratio), or through the Print.Width
and
Print.Height
options. The maximum image size is graphics hardware
dependent.
You can create simple MPEG animations by choosing MPEG as the format in
‘File->Export’: this allows you to loop over time steps or
post-processing data sets, or to change parameters according to
Print.Parameter
. To create fully customized animations or to use
different output formats (AVI, MP4, etc.) you should write a
script. Have a look at t8
: Post-processing and animations or
demos/post_processing/anim.script
for some examples.
Yes: dragging the mouse in a numeric input field slides the value! The left button moves one step per pixel, the middle by ‘10*step’, and the right button by ‘100*step’.
Yes: selecting the content of an input field, or lines in the message console (‘Tools->Message Console’), copies the selected text to the clipboard.
Next: Mesh module, Previous: General questions, Up: Frequently asked questions [Contents][Index]
Yes, but only with the OpenCASCADE kernel.
The default behavior of Gmsh is to check and suppress all duplicate entities (points, curves and surfaces) each time a transformation command is issued with the built-in CAD kernel. This can slow down things a lot if many transformations are performed. There are two solutions to this problem:
Geometry.AutoCoherence
option to 0. This will
prevent any automatic duplicate check/replacement. If you still need to
remove the duplicates entities, simply add Coherence;
at
strategic locations in your .geo
files (e.g. before the creation
of curve loops, etc.).
Use ‘Tools->Visibility’. This allows you to select elementary entities and physical groups, as well as mesh elements, in a variety of ways (in a list or tree browser, by tag, interactively, or per window).
Yes: with the OpenCASCADE kernel (SetFactory("OpenCASCADE");
),
load the file (Merge "file.step";
or
ShapeFromFile("file.step");
) and add the relevant scripting
commands after that to delete parts, create new parts or apply boolean
operators. See
e.g. demos/boolean/import.geo.
.geo
file?
You should not export STEP models as .geo
files. By
design, Gmsh never translates from one CAD format to another. The
“unrolled GEO” feature is there for unrolling complex GEO
scripts. While it can indeed export a limited subset of geometrical
entities created by other CAD kernels, it’s there only for debugging
purposes. If you want to modify a STEP model, see the previous question.
Define common geometrical objects and options in separate files or using
Macro
, reusable in all your problem definition structures. Or use
the features of your language of choice and the Gmsh API.
In Gmsh 4, some operations (Color
, Show
, Hide
,
BoundingBox
, Boundary
, PointsOf
, Periodic
,
In
embedding constraints, ..) are now applied directly on the
internal Gmsh model, instead of being handled at the level of the CAD
kernel. This implies a synchronization between the CAD kernel and the
Gmsh model. To minimize the number of synchronizations (which can become
costly for large models), you should always create your geometry first;
and use these commands once the geometry has been created.
Next: Solver module, Previous: Geometry module, Up: Frequently asked questions [Contents][Index]
Verify that the curves in the model do not self-intersect. If
‘Mesh.RandomFactor
* size of triangle / size of model’ approaches
machine accuracy, increase Mesh.RandomFactor
.
If everything fails file a bug report with the version of your operating system and the full geometry.
Verify that the surfaces in your model do not self-intersect or partially overlap. If they don’t, try the other 3D algorithms (‘Tool->Options->Mesh->General->3D algorithm’) or try to adapt the mesh element sizes in your input file so that the surface mesh better matches the geometrical details of the model.
If nothing works, file a bug report with the version of your operating system and the full geometry.
By default, if physical groups are defined, the output mesh only contains those elements that belong to physical entities. So to save only 3D elements, simply define one (or more) physical volume(s) and don’t define any physical surfaces, physical curves or physical points.
By default Gmsh saves all the geometrical entities and their associated mesh. In particular, since each geometry point is meshed with a point element, defined by a mesh node, the output file will contain one 0-D mesh element and one mesh node for each geometry point. To remove such elements/nodes from the mesh, simply define physical groups for the entities you want to save (see previous question).
IGES files do not contain the topology of the model, and tolerance problems can thus appear when the OpenCASCADE importer cannot identify two (close) curves as actually being identical.
The best solution is to not use IGES and use STEP instead. If you really have to use IGES, check that you don’t have duplicate curves (e.g. by displaying their tags in the GUI with ‘Tools->Options->Geometry->Visibility->Curve labels’). If there are duplicates, try to change the geometrical tolerance and sew the faces (see options in ‘Tools->Options->Geometry->General’).
Use ‘Optimize quality’ in the mesh menu.
The swapping algorithm is not very clever. Try to change the surface mesh a bit, or recombine your mesh to generate prisms or hexahedra instead of tetrahedra.
Yes, but only if pyramids need to be created on a single side of the quadrangular surface mesh.
No, this feature has been removed in Gmsh 2.0. You must use the standard entity tag instead.
Yes. You can achieve the same result by using the transfinite
algorithm with smoothing (e.g., with Mesh.Smoothing = 10
).
Yes, just choose the appropriate order in the mesh menu after the mesh
is completed. High-order optimization tools are also available in the
mesh menu. You can select the order on the command line with e.g.
-order 2
, and activcate high-order optimization with
-optimize_ho
.
Yes, you can import a surface mesh in any one of the supported mesh file formats, define a volume, and mesh it. For an example see demos/simple_geo/sphere-discrete.geo.
By design, Gmsh does not try to incorporate every possible definition of
boundary conditions or material properties—this is a job best left to
the solver. Instead, Gmsh provides a simple mechanism to tag groups of
elements, and it is up to the solver to interpret these tags as boundary
conditions, materials, etc. Associating tags with elements in Gmsh is
done by defining physical groups (Physical Points, Physical Curves,
Physical Surfaces and Physical Volumes). See the reference manual as
well as the tutorials (in particular t1
: Geometry basics, elementary entities, physical groups) for a detailed
description and some examples.
See “How can I display only selected parts of my model?”.
You can use ‘Tools->Clipping’ to clip the region of interest. You can define up to 6 clipping planes in Gmsh (i.e., enough to define a “cube” inside your model) and each plane can clip either the geometry, the mesh, the post-processing views, or any combination of the above. The clipping planes are defined using the four coefficients A,B,C,D of the equation A*x+B*y+C*y+D=0, which can be adjusted interactively by dragging the mouse in the input fields.
They measure the quality of the tetrahedra in a mesh:
For the exact definitions, see Geo/MElement.cpp. The graphs plot the the number of elements vs. the quality measure.
-format
option (e.g. gmsh
file.geo -format msh2 -2
).
.geo
script: add the line Mesh.MshFileVersion = x.y;
for any version number x.y
. You can also save this in your
default options.
gmsh::option::setNumber("Mesh.MshFileVersion", x.y)
.
As an alternative method, you can also not specify the format
explicitly, and just choose a filename with the .msh2
or
.msh4
extension.
Each numerical method has its own requirements: it might need neighboring elements connected by a node, an edge or a face; it might require a single layer or multiple layers; it should include elements of lower dimension (boundaries) or not, go across geometrical entities or mesh partitions or not, etc. Given the number of possibilities, generating the appropriate information is thus best performed in the numerical solver itself. The Gmsh API makes these computations easy: see for example demos/api/neighbors.py.
Edge/faces can be easily generated from the information already available in the file (i.e. nodes and elements), or through the Gmsh API: see for example demos/api/faces.cpp.
Next: Post-processing module, Previous: Mesh module, Up: Frequently asked questions [Contents][Index]
Gmsh uses the ONELAB interface (http://www.onelab.info) to interact with external solvers. See Solver module.
Using the Gmsh API, you can directly embed Gmsh in your own solver, use ONELAB for interactive parameter definition and modification, and create visualization data on the fly. See e.g. prepro.py, custom_gui.py, custom_gui.cpp.
Another (rather crude) approach if to launch the Gmsh app everytime you want to visualize something (a simple C program showing how to do this is given in utils/misc/callgmsh.c).
Yet another approach is to modify your program so that it can
communicate with Gmsh through ONELAB over a socket. Select ‘Always
listen to incoming connection requests’ in the Gmsh solver option panel
(or run gmsh with the -listen
command line option), and Gmsh will
always listen for your program on the given socket (or on the
Solver.SocketName
if no socket is specified).
Previous: Solver module, Up: Frequently asked questions [Contents][Index]
Use ‘Tools->Plugins->Cut Plane’.
Yes: first run ‘Tools->Plugins->Isosurface’ to extract the isosurface, then use ‘View->Export’ to save the new view.
Yes, with the CutMap plugin (set the ExtractVolume option to -1 or 1 to extract the negative or positive levelset).
If the views contain multiple time steps, you can press the ‘play’ button at the bottom of the graphic window, or change the time step by hand in the view option panel. You can also use the left and right arrow keys on your keyboard to change the time step in all visible views in real time.
If you want to loop through different views instead of time steps, you can use the ‘Loop through views instead of time steps’ option in the view option panel, or use the up and down arrow keys on your keyboard.
Load a vector view containing the displacement field, and set ‘Vector display’ to ‘Displacement’ in ‘View->Options->Aspect’. If the displacement is too small (or too large), you can scale it with the ‘Displacement factor’ option. (Remember that you can drag the mouse in all numeric input fields to slide the value!)
Another option is to use the ‘General transformation expressions’ (in View->Options->Offset) on a scalar view, with the displacement map selected as the data source.
Yes, there are several ways to do that.
The easiest is to load two views: the first one containing a displacement field (a vector view that will be used to deform the mesh), and the second one containing the field you want to display (this view has to contain the same number of elements as the displacement view). You should then set ‘Vector display’ to ‘Displacement’ in the first view, as well as set ‘Data source’ to point to the second view. (You might want to make the second view invisible, too. If you want to amplify or decrease the amount of deformation, just modify the ‘Displacement factor’ option.)
Another solution is to use the ‘General transformation expressions’ (in ‘View->Options->Offset’) on the field you want to display, with the displacement map selected as the data source.
And yet another solution is to use the Warp plugin.
Yes: load both the vector and the scalar fields (the two views must have the same number of elements) and, in the vector field options, select the scalar view in ‘Data source’.
Yes, using either the CutMap plugin (with the ‘dView’ option) or the Evaluate plugin.
You can save simple MPEG animations directly from the ‘File->Export’
menu. For other formats you should write a script. Have a look at
t8
: Post-processing and animations or
demos/post_processing/anim.script
for some examples.
Yes, by using either the “Force field” options in ‘Tools->Options->View->Visibility’, or by using ‘Tools->Plugins->MathEval’.
Yes, with the Evaluate plugin.
There can be several reasons:
Plugin(DecomposeinSimplex)
to transform all quads, hexas, prisms
and pyramids into triangles and tetrahedra).
Plugin(Triangulate)
to transform a
point cloud into a triangulated surface. In 3D you can use
Plugin(Tetrahedralize)
.
In any case, you can automatically remove all empty views with
‘View->Remove->Empty Views’ in the GUI, or with Delete Empty
Views;
in a script.
Use ‘Tools->Clipping’.
When viewing 3D scalar fields, you can also modify the colormap (‘Tools->Options->View->Map’) to make the iso-surfaces “transparent”: either by holding ‘Ctrl’ while dragging the mouse to draw the alpha channel by hand, or by using the ‘a’, ‘Ctrl+a’, ‘p’ and ‘Ctrl+p’ keyboard shortcuts.
Yet another (destructive) option is to use the ExtractVolume option in the CutSphere or CutPlane plugins.
If your dataset is constant per element make sure you don’t use the ‘Iso-values’ interval type in ‘Tools->Options->View->Range’.
Next: Copyright and credits, Previous: Frequently asked questions, Up: Gmsh [Contents][Index]
4.8.4 (April 28, 2021) : set current model in gmsh/model/add; small bug fixes. 4.8.3 (April 6, 2021): better handling of errors in inverse surface mapping; fixed Mesh.MedFileMinorVersion for MED 4; small bug fixes. 4.8.2 (March 27, 2021): fixed regression in OCC transforms; fixed cwrap API. 4.8.1 (March 21, 2021): improved performance when transforming many OCC entities; fixed regression in high-order meshing of surfaces with singular parametrizations; small bug fixes. 4.8.0 (March 2, 2021): new interactive and fully parametrizable definition of boundary conditions, materials, etc. through ONELAB variables; new API functions for creating trimmed BSpline/Bezier patches, perform raw triangulations and tetrehedralizations, get upward adjacencies, and create extruded boundary layers and automatic curve loops in built-in kernel; improved performance of high-order meshing of OCC models; improved handling of high resolution displays; new structured CGNS exporter; new transfinite Beta law; added support for embedded curves in HXT; added automatic conversion from partitioned MSH2 files to new partitioned entities; element groups can now be imported from UNV files; fixed order of Gauss quadrature for quads and hexas; code modernization (C++11); further uniformization of option names to match the documented terminology (Mesh.Point -> Mesh.Node, ...; old names are still accepted, but deprecated); deprecated Mesh.MinimumElementsPerTwoPi: set value directly to Mesh.MeshSizeFromCurvature instead; Python and Julia APIs now also define "snake case" aliases for all camelCase function names; small bug fixes and improvements. * Incompatible API changes: new optional arguments to mesh/classifySurfaces, occ/addBSplineSurface, occ/addBezierSurface, occ/addPipe and view/probe; renamed mesh/getEdgeNumber as mesh/getEdges 4.7.1 (November 16, 2020): small bug fixes and improvements. 4.7.0 (November 5, 2020): API errors now throw exceptions with the last error message (instead of an integer error code); API functions now print messages on the terminal by default, and throw exceptions on all errors unless in interactive mode; new API functions to retrieve "homogeneous" model-based data (for improved Python performance), to set interpolation matrices for high-order datasets, to assign "automatic" transfinite meshing constraints and to pass native (C++, C, Python or Julia) mesh size callback; added option to save high-order periodic nodes info; added support for scripted window splitting; improved VTK reader; new MatrixOfInertia command; added support for Unicode command line arguments on Windows; uniformized commands, options and field option names to match the documented terminology (CharacteristicLength -> MeshSize, geometry Line -> Curve, ...; old names are still accepted, but deprecated); improved handling of complex periodic cases; removed bundled Mmg3D and added support for stock Mmg 5; Gmsh now requires C++11 and CMake 3.1, and uses Eigen by default instead of Blas/Lapack for dense linear algebra; small bug fixes. * Incompatible API changes: new optional argument to geo/addCurveLoop 4.6.0 (June 22, 2020): new options to only generate initial 2D or 3D meshes (without node insertion), and to only mesh non-meshed entities; added ability to only remesh parts of discrete models; added support for mesh size fields and embedded points and surfaces in HXT; improved reparametrization and partitioning code; new OCC API functions to reduce the number of synchronizations for complex models; new OCC spline surface interfaces; new functions and options to control the first tag of entities, nodes and elements; fixed duplicated entities in STEP output; improved mesh subdivision and high-order pipeline; MED output now preserves node and element tags; small bug fixes. * Incompatible API changes: new optional arguments to mesh/clear, mesh/createTopology, mesh/createGeometry, occ/addThruSections, mesh/getPeriodicNodes; new arguments to mesh/getBasisFunctions; removed mesh/preallocateBasisFunctions, mesh/precomputeBasisFunctions and mesh/getBasisFunctionsForElements; renamed occ/setMeshSize as occ/mesh/setSize 4.5.6 (March 30, 2020): better calculation of OCC bounding boxes using STL; API tutorials; small bug fixes. 4.5.5 (March 21, 2020): tooltips in GUI to help discovery of scripting options; fixed MED IO of high-order elements; fixed OCC attribute search by bounding box; fix parsing of mac-encoded scripts; new RecombineMesh command; added support for extrusion of mixed-dimension entities with OCC; small bug fixes. 4.5.4 (February 29, 2020): periodic mesh optimization now ensures that the master mesh is not modified; code cleanup; small bug fixes. 4.5.3 (February 22, 2020): improved positioning of corresponding nodes on periodic entities; improved LaTeX output; improved curve splitting in reparametrization; new binary PLY reader; small compilation fixes. 4.5.2 (January 30, 2020): periodic meshes now obey reorientation constraints; physical group definitions now follow compound meshing constraints; small bug fixes and improvements. 4.5.1 (December 28, 2019): new Min and Max commands in .geo files; Mesh.MinimumCirclePoints now behaves the same with all geometry kernels; fixed issue with UTF16-encoded home directories on Windows. 4.5.0 (December 21, 2019): changed default 2D meshing algorithm to Frontal-Delaunay; new compound Spline/BSpline commands; new MeshSizeFromBoundary command; new CGNS importer/exporter; new X3D exporter for geometries and meshes; improved surface mesh reclassification; new separate option to govern curvature adapted meshes (Mesh.MinimumElementsPerTwoPi and "-clcurv val"); improved handling of anisotropic surface meshes in 3D Delaunay; improved high-order periodic meshing; improved 2D boolean unions; file chooser type is now changeable at runtime; FLTK GUI can now be created and destroyed at will through the API; fixed regression in MeshAdapt for non-periodic surfaces with singularities; combining views now copies options; added API support for mesh compounds, per-surface mesh algorithm and mesh size from boundary; renamed plugin AnalyseCurvedMesh to AnalyseMeshQuality; fixed regression for built-in kernel BSplines on non-flat geometries (Sphere, PolarSphere); small fixes and improvements. * Incompatible API changes: removed mesh/smooth (now handled by mesh/optimize like all other mesh optimizers); renamed logger/time to logger/getWallTime and logger/cputime to logger/getCpuTime; new arguments to mesh/optimize, mesh/getElementProperties and occ/healShapes; added optional argument to mesh/classifySurfaces and view/combine. 4.4.1 (July 25, 2019): small improvements (transfinite with degenerate curves, renumbering for some mesh formats, empty MSH file sections, tunable accuracy of compound meshes) and bug fixes (ellipse < pi, orientation and reclassification of compound parts, serendip pyramids, periodic MeshAdapt robustness, invalidate cache after mesh/addNodes). 4.4.0 (July 1, 2019): new STL remeshing workflow (with new ClassifySurfaces command in .geo files); added API support for color options, mesh optimization, recombination, smoothing and shape healing; exposed additional METIS options; improved support for periodic entities (multiple curves with the same start/end points, legacy MSH2 format, periodic surfaces with embedded entities); added mesh renumbering also after interactive mesh modifications; improved support for OpenCASCADE ellipse arcs; new interactive filter in visibility window; flatter GUI; small bug fixes. * Incompatible API changes: mesh/getJacobians and mesh/getBasisFunctions now take integration points explicitely; mesh/setNodes and mesh/setElements have been replaced by mesh/addNodes and mesh/addElements; added optional arguments to mesh/classifySurfaces and occ/addSurfaceLoop; changed arguments of occ/addEllipseArc to follow geo/addEllipseArc. 4.3.0 (April 19, 2019): improved meshing of surfaces with singular parametrizations; added API support for aliasing and combining views, copying view options, setting point coordinates, extruding built-in CAD entities along normals and retrieving mass, center of mass and inertia from OpenCASCADE CAD entities; fixed regression introduced in 4.1.4 that could lead to non-deterministic 2D meshes; small bug fixes. * Incompatible API changes: added optional arguments to mesh/getNodes and mesh/getElementByCoordinates 4.2.3 (April 3, 2019): added STL export by physical surface; added ability to remove embedded entities; added handling of boundary entities in addDiscreteEntity; small bug fixes. 4.2.2 (March 13, 2019): fixed regression in reading of extruded meshes; added ability to export one solid per surface in STL format. 4.2.1 (March 7, 2019): fixed regression for STEP files without global compound shape; added support for reading IGES labels and colors; improved search for shared library in Python and Julia modules; improved Plugin(MeshVolume); updates to the reference manual. 4.2.0 (March 5, 2019): new MSH4.1 revision of the MSH file format, with support for size_t node and element tags (see the reference manual for detailed changes); added support for reading STEP labels and colors with OCC CAF; changed default "Geometry.OCCTargetUnit" value to none (i.e. use STEP file coordinates as-is, without conversion); improved high-order mesh optimization; added ability to import groups of nodes from MED files; enhanced Plugin(Distance) and Plugin(SimplePartition); removed unmaintained plugins; removed default dependency on PETSc; small improvements and bug fixes. * Incompatible API changes: changed type of node and element tags from int to size_t to support (very) large meshes; changed logger/start, mesh/getPeriodicNodes and mesh/setElementsByType. 4.1.5 (February 14, 2019): improved OpenMP parallelization, STL remeshing, mesh partitioning and high-order mesh optimization; added classifySurfaces in API; bug fixes. 4.1.4 (February 3, 2019): improved ghost cell I/O; added getGhostElements, relocateNodes, getElementType, getElementFaceNodes, getElementEdgeNodes functions in API; small improvements and bug fixes. 4.1.3 (January 23, 2019): improved quad meshing; new options for automatic full-quad meshes; save nodesets also for physical points (Abaqus, Tochnog); new getPartitions, unpartition and removePhysicalName functions in API; small bug fixes. 4.1.2 (January 21, 2019): fixed full-quad subdivision if Mesh.SecondOrderLinear is set; fixed packing of parallelograms regression in 4.1.1. 4.1.1 (January 20, 2019): added support for general affine transformations with OpenCASCADE kernel; improved handling of boolean tolerance (snap vertices); faster crossfield calculation by default (e.g. for Frontal-Delauany for quads algorithm); fixed face vertices for PyramidN; renamed ONELAB "Action" and "Button" parameters "ONELAB/Action" and "ONELAB/Button"; added support for actions on any ONELAB button; added API functions for selections in user interface. 4.1.0 (January 13, 2019): improved ONELAB and Fltk support in API; improved renumbering of mesh nodes/elements; major code refactoring. * Incompatible API changes: changed onelab/get. 4.0.7 (December 9, 2018): fixed small memory leaks; removed unused code. 4.0.6 (November 25, 2018): moved private API wrappers to utils/wrappers; improved Gmsh 3 compatibility for high-order periodic meshes; fixed '-v 0' not being completely silent; fixed rendering of image textures on some OSes; small compilation fixes. 4.0.5 (November 17, 2018): new automatic hybrid mesh generation (pyramid layer) when 3D Delaunay algorithm is applied to a volume with quadrangles on boundary; improved robustness of 2D MeshAdapt algorithm; bug fixes. 4.0.4 (October 19, 2018): fixed physical names regression in 4.0.3. 4.0.3 (October 18, 2018): bug fixes. 4.0.2 (September 26, 2018): added support for creating MED files with specific MED (minor) version; small bug fixes. 4.0.1 (September 7, 2018): renumber mesh nodes/elements by default; new SendToServer command for nodal views; added color and visibility handling in API; small bug fixes. 4.0.0 (August 22, 2018): new C++, C, Python and Julia API; new MSH4 format; new mesh partitioning code based on Metis 5; new 3D tetrahedralization algorithm as default; new workflow for remeshing (compound entities as meshing constraints, CreateGeometry for mesh reparametrization); added support for general BSplines, fillets and chamfers with OpenCASCADE kernel and changed default BSpline parameters with the built-in kernel to match OpenCASCADE's; STEP files are now be default interpreted in MKS units (see Geometry.OCCTargetUnit); improved meshing of surfaces with singular parametrizations (spheres, etc.); uniformized entity naming conventions (line/curve, vertex/node, etc.); generalized handling of "all" entities in geo file (using {:} notation); added support for creating LSDYNA mesh files; removed old CAD creation factory (GModelFactory), old reparametrization code (G{Edge, Face, Region}Compound) and old partitioning code (Metis 4 and Chaco); various cleanups, bug fixes and enhancements. 3.0.6 (November 5, 2017): improved meshing of spheres; improved handling of mesh size constraints with OpenCASCADE kernel; implemented "Coherence" for OpenCASCADE kernel (shortcut for BooleanFragments); added GAMBIT Neutral File export; small improvements and bug fixes. 3.0.5 (September 6, 2017): bug fixes. 3.0.4 (July 28, 2017): moved vorometal code to plugin; OpenMP improvements; bug fixes. 3.0.3 (June 27, 2017): new element quality measures; Block->Box; minor fixes. 3.0.2 (May 13, 2017): improved handling of meshing constraints and entity numbering after boolean operations; improved handling of fast coarseness transitions in MeshAdapt; new TIKZ export; small bug fixes. 3.0.1 (April 14, 2017): fixed OpenCASCADE plane surfaces with holes. 3.0.0 (April 13, 2017): new constructive solid geometry features and boolean operations using OpenCASCADE; improved graphical user interface for interactive, parametric geometry construction; new or modified commands in .geo files: SetFactory, Circle, Ellipse, Wire, Surface, Sphere, Block, Torus, Rectangle, Disk, Cylinder, Cone, Wedge, ThickSolid, ThruSections, Ruled ThruSections, Fillet, Extrude, BooleanUnion, BooleanIntersection, BooleanDifference, BooleanFragments, ShapeFromFile, Recursive Delete, Unique; "Surface" replaces the deprecated "Ruled Surface" command; faster 3D tetrahedral mesh optimization enabled by default; major code refactoring and numerous bug fixes. 2.16.0 (January 3, 2017): small improvements (list functions, second order hexes for MED, GUI) and bug fixes. 2.15.0 (December 4, 2016): fixed several regressions (multi-file partitioned grid export, mesh subdivision, old compound mesher); improved 2D boundary layer field & removed non-functional 3D boundary layer field; faster rendering of large meshes. 2.14.1 (October 30, 2016): fixed regression in periodic meshes; small bug fixes and code cleanups. 2.14.0 (October 9, 2016): new Tochnog file format export; added ability to remove last command in scripts generated interactively; ONELAB 1.3 with usability and performance improvements; faster "Coherence Mesh". 2.13.2 (August 18, 2016)): small improvements (scale labels, periodic and high-order meshes) and bug fixes. 2.13.1 (July 15, 2016): small bug fixes. 2.13.0 (July 11, 2016): new ONELAB 1.2 protocol with native support for lists; new experimental 3D boundary recovery code and 3D refinement algorithm; better adaptive visualization of quads and hexahedra; fixed several regressions introduced in 2.12. 2.12.0 (March 5, 2016): improved interactive definition of physical groups and handling of ONELAB clients; improved full quad algorithm; added support for list of strings, trihedra elements and X3D format; improved message console; new colormaps; various bugs fixes and small improvements all over. 2.11.0 (November 7, 2015): new Else/ElseIf commands; new OptimizeMesh command; Plugin(ModifyComponents) replaces Plugin(ModifyComponent); new VTK and X3D outputs; separate 0/Ctrl+0 shortcuts for geometry/full model reload; small bug fixes in homology solver, handling of embedded entities, and Plugin(Crack). 2.10.1 (July 30, 2015): minor fixes. 2.10.0 (July 21, 2015): improved periodic meshing constraints; new Physical specification with both label and numeric id; images can now be used as glyphs in post-processing views, using text annotations with the `file://' prefix; Views can be grouped and organized in subtrees; improved visibility browser navigation; geometrical entities and post-processing views can now react to double-clicks, via new generic DoubleClicked options; new Get/SetNumber and Get/SetString for direct access to ONELAB variables; small bug fixes and code cleanups. 2.9.3 (April 18, 2015): updated versions of PETSc/SLEPc and OpenCASCADE/OCE libraries used in official binary builds; new Find() command; miscellaneous code cleanups and small fixes. 2.9.2 (March 31, 2015): added support for extrusion of embedded points/curves; improved hex-dominant algorithm; fixed crashes in quad algorithm; fix regression in MED reader introduced in 2.9.0; new dark interface mode. 2.9.1 (March 18, 2015): minor bug fixes. 2.9.0 (March 12, 2015): improved robustness of spatial searches (extruded meshes, geometry coherence); improved reproductibility of 2D and 3D meshes; added support for high resolution ("retina") graphics; interactive graph point commands; on-the-fly creation of onelab clients in scripts; general periodic meshes using afine transforms; scripted selection of entities in bounding boxes; extended string and list handling functions; many small improvements and bug fixes. 2.8.5 (Jul 9, 2014): improved stability and error handling, better Coherence function, updated onelab API version and inline parameter definitions, new background image modes, more robust Triangulate/Tetrahedralize plugins, new PGF output, improved support for string~index variable names in parser, small improvements and bug fixes all over the place. 2.8.4 (Feb 7, 2014): better reproductibility of 2D meshes; new mandatory 'Name' attribute to define onelab variables in DefineConstant[] & co; new -setnumber/-setstring command line arguments; small improvements and bug fixes. 2.8.3 (Sep 27, 2013): new quick access menu and multiple view selection in GUI; enhanced animation creation; many small enhancements and bug fixes. 2.8.2 (Jul 16, 2013): improved high order tools interface; minor bug fixes. 2.8.1 (Jul 11, 2013): improved compound surfaces and transfinite arrangements. 2.8.0 (Jul 8, 2013): improved Delaunay point insertion; fixed mesh orientation of plane surfaces; fixed mesh size prescribed at embedded points; improved display of vectors at COG; new experimental text string display engines; improved fullscreen mode; access time/step in transformations; new experimental features: AdaptMesh and Surface In Volume; accept unicode file paths on Windows; compilation and bug fixes. 2.7.1 (May 11, 2013): improved Delaunay point insertion; updated onelab; better Abaqus and UNV export; small bug and compilation fixes. 2.7.0 (Mar 9, 2013): new single-window GUI, with dynamically customizable widget tree; faster STEP/BRep import; arbitrary size image export; faster 2D Delaunay/Frontal algorithms; full option viewer/editor; many bug fixes. 2.6.1 (Jul 15, 2012): minor improvements and bug fixes. 2.6.0 (Jun 19, 2012): new quadrilateral meshing algorithms (Blossom and Delaunay-Frontal for quads); new solver module based on ONELAB project (requires FLTK 1.3); new tensor field visualization modes (eigenvectors, ellipsoid, etc.); added support for interpolation schemes in .msh file; added support for MED3 format; rescale viewport around visible entities (shift+1:1 in GUI); unified post-processing field export; new experimental stereo+camera visualization mode; added experimental BAMG & Mmg3D support for anisotropic mesh generation; new OCC cut & merge algorithm imported from Salome; new ability to connect extruded meshes to tetrahedral grids using pyramids; new homology solver; Abaqus (INP) mesh export; new Python and Java wrappers; bug fixes and small improvements all over the place. 2.5.0 (Oct 15, 2010): new compound geometrical entities (for remeshing and/or trans-patch meshing); improved mesh reclassification tool; new client/server visualization mode; new ability to watch a pattern of files to merge; new integrated MPEG export; new option to force the type of views dynamically; bumped mesh version format to 2.2 (small change in the meaning of the partition tags; this only affects partitioned (i.e. parallel) meshes); renamed several post-processing plugins (as well as plugin options) to make them easier to understand; many bug fixes and usability improvements all over the place. 2.4.2 (Sep 21, 2009): solver code refactoring + better IDE integration. 2.4.1 (Sep 1, 2009): fixed surface mesh orientation bug introduced in 2.4.0; mesh and graphics code refactoring, small usability enhancements and bug fixes. 2.4.0 (Aug 22, 2009): switched build system to CMake; optionally copy transfinite mesh constraints during geometry transformations; bumped mesh version format to 2.1 (small change in the $PhysicalNames section, where the group dimension is now required); ported most plugins to the new post-processing API; switched from MathEval to MathEx and Flu_Tree_Browser to Fl_Tree; small bug fixes and improvements all over the place. 2.3.1 (Mar 18, 2009): removed GSL dependency (Gmsh now simply uses Blas and Lapack); new per-window visibility; added support for composite window printing and background images; fixed string option affectation in parser; fixed surface mesh orientation for OpenCASCADE models; fixed random triangle orientations in Delaunay and Frontal algorithms. 2.3.0 (Jan 23, 2009): major graphics and GUI code refactoring; new full-quad/hexa subdivision algorithm; improved automatic transfinite corner selection (now also for volumes); improved visibility browser; new automatic adaptive visualization for high-order simplices; modified arrow size, clipping planes and transform options; many improvements and bug fixes all over the place. 2.2.6 (Nov 21, 2008): better transfinite smoothing and automatic corner selection; fixed high order meshing crashes on Windows and Linux; new uniform mesh refinement (thanks Brian!); fixed various other small bugs. 2.2.5 (Oct 25, 2008): Gmsh now requires FLTK 1.1.7 or above; various small improvements (STL and VTK mesh I/O, Netgen upgrade, Visual C++ support, Fields, Mesh.{Msh,Stl,...}Binary changed to Mesh.Binary) and bug fixes (pyramid interpolation, Chaco crashes). 2.2.4 (Aug 14, 2008): integrated Metis and Chaco mesh partitioners; variables can now be deleted in geo files; added support for point datasets in model-based postprocessing views; small bug fixes. 2.2.3 (Jul 14, 2008): enhanced clipping interface; API cleanup; fixed various bugs (Plugin(Integrate), high order meshes, surface info crash). 2.2.2 (Jun 20, 2008): added geometrical transformations on volumes; fixed bug in high order mesh generation. 2.2.1 (Jun 15, 2008): various small improvements (adaptive views, GUI, code cleanup) and bug fixes (high order meshes, Netgen interface). 2.2.0 (Apr 19, 2008): new model-based post-processing backend; added MED I/O for mesh and post-processing; fixed BDF vertex ordering for 2nd order elements; replaced Mesh.ConstrainedBackgroundMesh with Mesh.CharacteristicLength{FromPoints,ExtendFromBoundary}; new Fields interface; control windows are now non-modal by default; new experimental 2D frontal algorithm; fixed various bugs. 2.1.1 (Mar 1, 2008): small bug fixes (second order meshes, combine views, divide and conquer crash, ...). 2.1.0 (Feb 23, 2008): new post-processing database; complete rewrite of post-processing drawing code; improved surface mesh algorithms; improved STEP/IGES/BREP support; new 3D mesh optimization algorithm; new default native file choosers; fixed 'could not find extruded vertex' in extrusions; many improvements and bug fixes all over the place. 2.0.8 (Jul 13, 2007): unused vertices are not saved in mesh files anymore; new plugin GUI; automatic GUI font size selection; renamed Plugin(DecomposeInSimplex) into Plugin(MakeSimplex); reintroduced enhanced Plugin(SphericalRaise); clarified meshing algo names; new option to save groups of nodes in UNV meshes; new background mesh infrastructure; many small improvements and small bug fixes. 2.0.7 (Apr 3, 2007): volumes can now be defined from external CAD surfaces; Delaunay/Tetgen algorithm is now used by default when available; re-added support for Plot3D structured mesh format; added ability to export external CAD models as GEO files (this only works for the limited set of geometrical primitives available in the GEO language, of course--so trying to convert e.g. a trimmed NURBS from a STEP file into a GEO file will fail); "lateral" entities are now added at the end of the list returned by extrusion commands; fixed various bugs. 2.0.0 (Feb 5, 2007): new geometry and mesh databases, with support for STEP and IGES import via OpenCASCADE; complete rewrite of geometry and mesh drawing code; complete rewrite of mesh I/O layer (with new native binary MSH format and support for import/export of I-deas UNV, Nastran BDF, STL, Medit MESH and VRML 1.0 files); added support for incomplete second order elements; new 2D and 3D meshing algorithms; improved integration of Netgen and TetGen algorithms; removed anisotropic meshing algorithm (as well as attractors); removed explicit region number specification in extrusions; option changes in the graphical interface are now applied instantaneously; added support for offscreen rendering using OSMesa; added support for SVG output; added string labels for Physical entities; lots of other improvements all over the place. 1.65 (May 15, 2006): new Plugin(ExtractEdges); fixed compilation errors with gcc4.1; replaced Plugin(DisplacementRaise) and Plugin(SphericalRaise) with the more flexible Plugin(Warp); better handling of discrete curves; new Status command in parser; added option to renumber nodes in .msh files (to avoid holes in the numbering sequence); fixed 2 special cases in quad->prism extrusion; fixed saving of 2nd order hexas with negative volume; small bug fixes and cleanups. 1.64 (Mar 18, 2006): Windows versions do no depend on Cygwin anymore; various bug fixes and cleanups. 1.63 (Feb 01, 2006): post-processing views can now be exported as meshes; improved background mesh handling (a lot faster, and more accurate); improved support for input images; new Plugin(ExtractElements); small bug fixes and enhancements. 1.62 (Jan 15, 2006): new option to draw color gradients in the background; enhanced perspective projection mode; new "lasso" selection mode (same as "lasso" zoom, but in selection mode); new "invert selection" button in the visibility browser; new snapping grid when adding points in the GUI; nicer normal smoothing; new extrude syntax (old syntax still available, but deprecated); various small bug fixes and enhancements. 1.61 (Nov 29, 2005): added support for second order (curved) elements in post-processor; new version (1.4) of post-processing file formats; new stippling options for 2D plots; removed limit on allowed number of files on command line; all "Combine" operations are now available in the parser; changed View.ArrowLocation into View.GlyphLocation; optimized memory usage when loading many (>1000) views; optimized loading and drawing of line meshes and 2D iso views; optimized handling of meshes with large number of physical entities; optimized vertex array creation for large post-processing views on Windows/Cygwin; removed Discrete Line and Discrete Surface commands (the same functionality can now be obtained by simply loading a mesh in .msh format); fixed coloring by mesh partition; added option to light wireframe meshes and views; new "mesh statistics" export format; new full-quad recombine option; new Plugin(ModulusPhase); hexas and prisms are now always saved with positive volume; improved interactive entity selection; new experimental Tetgen integration; new experimental STL remeshing algorithm; various small bug fixes and improvements. 1.60 (Mar 15, 2005): added support for discrete curves; new Window menu on Mac OS X; generalized all octree-based plugins (CutGrid, StreamLines, Probe, etc.) to handle all element types (and not only scalar and vector triangles+tetrahedra); generalized Plugin(Evaluate), Plugin(Extract) and Plugin(Annotate); enhanced clipping plane interface; new grid/axes/rulers for 3D post-processing views (renamed the AbscissaName, NbAbscissa and AbscissaFormat options to more general names in the process); better automatic positioning of 2D graphs; new manipulator dialog to specify rotations, translations and scalings "by hand"; various small enhancements and bug fixes. 1.59 (Feb 06, 2005): added support for discrete (triangulated) surfaces, either in STL format or with the new "Discrete Surface" command; added STL and Text output format for post-processing views and STL output format for surface meshes; all levelset-based plugins can now also compute isovolumes; generalized Plugin(Evaluate) to handle external view data (based on the same or on a different mesh); generalized Plugin(CutGrid); new plugins (Eigenvalues, Gradient, Curl, Divergence); changed default colormap to match Matlab's "Jet" colormap; new transformation matrix option for views (for non-destructive rotations, symmetries, etc.); improved solver interface to keep the GUI responsive during solver calls; new C++ and Python solver examples; simplified Tools->Visibility GUI; transfinite lines with "Progression" now allow negative line numbers to reverse the progression; added ability to retrieve Gmsh's version number in the parser (to help write backward compatible scripts); fixed white space in unv mesh output; fixed various small bugs. 1.58 (Jan 01, 2005): fixed UNIX socket interface on Windows (broken by the TCP solver patch in 1.57); bumped version number of default post-processing file formats to 1.3 (the only small modification is the handling of the end-of-string character for text2d and text3d objects in the ASCII format); new File->Rename menu; new colormaps+improved colormap handling; new color+min/max options in views; new GetValue() function to ask for values interactively in scripts; generalized For/EndFor loops in parser; new plugins (Annotate, Remove, Probe); new text attributes in views; renamed some shortcuts; fixed TeX output for large scenes; new option dialogs for various output formats; fixed many small memory leaks in parser; many small enhancements to polish the graphics and the user interface. 1.57 (Dec 23, 2004): generalized displacement maps to display arbitrary view types; the arrows representing a vector field can now also be colored by the values from other scalar, vector or tensor fields; new adaptive high order visualization mode; new options (Solver.SocketCommand, Solver.NameCommand, View.ArrowSizeProportional, View.Normals, View.Tangents and General.ClipFactor); fixed display of undesired solver plugin popups; enhanced interactive plugin behavior; new plugins (HarmonicToTime, Integrate, Eigenvectors); tetrahedral mesh file reading speedup (50% faster on large meshes); large memory footprint reduction (up to 50%) for the visualization of triangular/tetrahedral meshes; the solver interface now supports TCP/IP connections; new generalized raise mode (allows to use complex expressions to offset post-processing maps); upgraded Netgen kernel to version 4.4; new optional TIME list in parsed views to specify the values of the time steps; several bug fixes in the Elliptic mesh algorithm; various other small bug fixes and enhancements. 1.56 (Oct 17, 2004): new post-processing option to draw a scalar view raised by a displacement view without using Plugin(DisplacementRaise) (makes drawing arbitrary scalar fields on deformed meshes much easier); better post-processing menu (arbitrary number of views+scrollable+show view number); improved view->combine; new horizontal post-processing scales; new option to draw the mesh nodes per element; views can now also be saved in "parsed" format; fixed various path problems on Windows; small bug fixes. 1.55 (Aug 21, 2004): added background mesh support for Triangle; meshes can now be displayed using "smoothed" normals (like post-processing views); added GUI for clipping planes; new interactive clipping/cutting plane definition; reorganized the Options GUI; enhanced 3D iso computation; enhanced lighting; many small bug fixes. 1.54 (Jul 03, 2004): integrated Netgen (3D mesh quality optimization + alternative 3D algorithm); Extrude Surface now always automatically creates a new volume (in the same way Extrude Point or Extrude Line create new lines and surfaces, respectively); fixed UNV output; made the "Layers" region numbering consistent between lines, surfaces and volumes; fixed home directory problem on Win98; new Plugin(CutParametric); the default project file is now created in the home directory if no current directory is defined (e.g., when double-clicking on the icon on Windows/Mac); fixed the discrepancy between the orientation of geometrical surfaces and the associated surface meshes; added automatic orientation of surfaces in surface loops; generalized Plugin(Triangulate) to handle vector and tensor views; much nicer display of discrete iso-surfaces and custom ranges using smooth normals; small bug fixes and cleanups. 1.53 (Jun 04, 2004): completed support for second order elements in the mesh module (line, triangles, quadrangles, tetrahedra, hexahedra, prisms and pyramids); various background mesh fixes and enhancements; major performance improvements in mesh and post-processing drawing routines (OpenGL vertex arrays for tri/quads); new Plugin(Evaluate) to evaluate arbitrary expressions on post-processing views; generalized Plugin(Extract) to handle any combination of components; generalized "Coherence" to handle transfinite surface/volume attributes; plugin options can now be set in the option file (like all other options); added "undo" capability during geometry creation; rewrote the contour guessing routines so that entities can be selected in an arbitrary order; Mac users can now double click on geo/msh/pos files in the Finder to launch Gmsh; removed support for FLTK 1.0; rewrote most of the code related to quadrangles; fixed 2d elliptic algorithm; removed all OpenGL display list code and options; fixed light positioning; new BoundingBox command to set the bounding box explicitly; added support for inexpensive "fake" transparency mode; many code cleanups. 1.52 (May 06, 2004): new raster ("bitmap") PostScript/EPS/PDF output formats; new Plugin(Extract) to extract a given component from a post-processing view; new Plugin(CutGrid) and Plugin(StreamLines); improved mesh projection on non-planar surfaces; added support for second order tetrahedral elements; added interactive control of element order; refined mesh entity drawing selection (and renamed most of the corresponding options); enhanced log scale in post-processing; better font selection; simplified View.Raise{X,Y,Z} by removing the scaling; various bug fixes (default postscript printing mode, drawing of 3D arrows/cylinders on Linux, default home directory on Windows, default initial file browser directory, extrusion of points with non-normalized axes of rotation, computation of the scene bounding box in scripts, + the usual documentation updates). 1.51 (Feb 29, 2004): initial support for visualizing mesh partitions; integrated version 2.0 of the MSH mesh file format; new option to compute post-processing ranges (min/max) per time step; Multiple views can now be combined into multi time step ones (e.g. for programs that generate data one time step at a time); new syntax: #var[] returns the size of the list var[]; enhanced "gmsh -convert"; temporary and error files are now created in the home directory to avoid file permission issues; new 3D arrows; better lighting support; STL facets can now be converted into individual geometrical surfaces; many other small improvements and bug fixes (multi timestep tensors, color by physical entity, parser cleanup, etc.). 1.50 (Dec 06, 2003): small changes to the visibility browser + made visibility scriptable (new Show/Hide commands); fixed (rare) crash when deleting views; split File->Open into File->Open and File->New to behave like most other programs; Mac versions now use the system menu bar by default (if possible); fixed bug leading to degenerate and/or duplicate tetrahedra in extruded meshes; fixed crash when reloading sms meshes. 1.49 (Nov 30, 2003): made Merge, Save and Print behave like Include (i.e., open files in the same directory as the main project file if the path is relative); new Plugin(DecomposeInSimplex); new option View.AlphaChannel to set the transparency factor globally for a post-processing view; new "Combine Views" command; various bug fixes and cleanups. 1.48 (Nov 23, 2003): new DisplacementRaise plugin to plot arbitrary fields on deformed meshes; generalized CutMap, CutPlane, CutSphere and Skin plugins to handle all kinds of elements and fields; new "Save View[n]" command to save views from a script; many small bug fixes (configure tests for libpng, handling of erroneous options, multi time step scalar prism drawings, copy of surface mesh attributes, etc.). 1.47 (Nov 12, 2003): fixed extrusion of surfaces defined by only two curves; new syntax to retrieve point coordinates and indices of entities created through geometrical transformations; new PDF and compressed PostScript output formats; fixed numbering of elements created with "Extrude Point/Line"; use $GMSH_HOME as home directory if defined. 1.46 (Aug 23, 2003): fixed crash for very long command lines; new options for setting the displacement factor and Triangle's parameters + renamed a couple of options to more sensible names (View.VectorType, View.ArrowSize); various small bug fixes; documentation update. 1.45 (Jun 14, 2003): small bug fixes (min/max computation for tensor views, missing physical points in read mesh, "jumping" geometry during interactive manipulation of large models, etc.); variable definition speedup; restored support for second order elements in one- and two-dimensional meshes; documentation updates. 1.44 (Apr 21, 2003): new reference manual; added support for PNG output; fixed small configure script bugs. 1.43 (Mar 28, 2003): fixed solver interface problem on Mac OS X; new option to specify the interactive rotation center (default is now the pseudo "center of gravity" of the object, instead of (0,0,0)). 1.42 (Mar 19, 2003): suppressed the automatic addition of a ".geo" extension if the file given on the command line is not recognized; added missing Layer option for Extrude Point; fixed various small bugs. 1.41 (Mar 04, 2003): Gmsh is now licensed under the GNU General Public License; general code cleanup (indent). 1.40 (Feb 26, 2003): various small bug fixes (mainly GSL-related). 1.39 (Feb 23, 2003): removed all non-free routines; more build system work; implemented Von-Mises tensor display for all element types; fixed small GUI bugs. 1.38 (Feb 17, 2003): fixed custom range selection for 3D iso graphs; new build system based on autoconf; new image reading code to import bitmaps as post-processing views. 1.37 (Jan 25, 2003): generalized smoothing and cuts of post-processing views; better Windows integration (solvers, external editors, etc.); small bug fixes. 1.36 (Nov 20, 2002): enhanced view duplication (one can now use "Duplicata View[num]" in the input file); merged all option dialogs in a new general option window; enhanced discoverability of the view option menus; new 3D point and line display; many small bug fixes and enhancements ("Print" format in parser, post-processing statistics, smooth normals, save window positions, restore default options, etc.). 1.35 (Sep 11, 2002): graphical user interface upgraded to FLTK 1.1 (tooltips, new file chooser with multiple selection, full keyboard navigation, cut/paste of messages, etc.); colors can be now be directly assigned to mesh entities; initial tensor visualization; new keyboard animation (right/left arrow for time steps; up/down arrow for view cycling); new VRML output format for surface meshes; new plugin for spherical elevation plots; new post-processing file format (version 1.2) supporting quadrangles, hexahedra, prisms and pyramids; transparency is now enabled by default for post-processing plots; many small bug fixes (read mesh, ...). 1.34 (Feb 18, 2002): improved surface mesh of non-plane surfaces; fixed orientation of elements in 2D anisotropic algorithm; minor user interface polish and additions (mostly in post-processing options); various small bug fixes. 1.33 (Jan 24, 2002): new parameterizable solver interface (allowing up to 5 user-defined solvers); enhanced 2D aniso algorithm; 3D initial mesh speedup. 1.32 (Oct 04, 2001): new visibility browser; better floating point exception checks; fixed infinite looping when merging meshes in project files; various small clean ups (degenerate 2D extrusion, view->reload, ...). 1.31 (Nov 30, 2001): corrected ellipses; PostScript output update (better shading, new combined PS/LaTeX output format); more interface polish; fixed extra memory allocation in 2D meshes; Physical Volume handling in unv format; various small fixes. 1.30 (Nov 16, 2001): interface polish; fix crash when extruding quadrangles. 1.29 (Nov 12, 2001): translations and rotations can now be combined in extrusions; fixed coherence bug in Extrude Line; various small bug fixes and additions. 1.28 (Oct 30, 2001): corrected the 'Using Progression' attribute for tranfinite meshes to actually match a real geometric progression; new Triangulate plugin; new 2D graphs (space+time charts); better performance of geometrical transformations (warning: the numbering of some automatically created entities has changed); new text primitives in post-processing views (file format updated to version 1.1); more robust mean plane computation and error checks; various other small additions and clean-ups. 1.27 (Oct 05, 2001): added ability to extrude curves with Layers/Recombine attributes; new PointSize/LineWidth options; fixed For/EndFor loops in included files; fixed error messages (line numbers+file names) in loops and functions; made the automatic removal of duplicate geometrical entities optional (Geometry.AutoCoherence=0); various other small bug fixes and clean-ups. 1.26 (Sep 06, 2001): enhanced 2D anisotropic mesh generator (metric intersections); fixed small bug in 3D initial mesh; added alternative syntax for built-in functions (for GetDP compatibility); added line element display; Gmsh now saves all the elements in the mesh if no physical groups are defined (or if Mesh.SaveAll=1). 1.25 (Sep 01, 2001): fixed bug with mixed recombined/non-recombined extruded meshes; Linux versions are now build with no optimization, due to bugs in gcc 2.95.X. 1.24 (Aug 30, 2001): fixed characteristic length interpolation for Splines; fixed edge swapping bug in 3D initial mesh; fixed degenerated case in geometrical extrusion (ruled surface with 3 borders); fixed generation of degenerated hexahedra and prisms for recombined+extruded meshes; added BSplines creation in the GUI; integrated Jonathan Shewchuk's Triangle as an alternative isotropic 2D mesh generator; added AngleSmoothNormals to control sharp edge display with smoothed normals; fixed random crash for lighted 3D iso surfaces. 1.23 (Aug, 2001): fixed duplicate elements generation + non-matching tetrahedra faces in 3D extruded meshes; better display of displacement maps; fixed interactive ellipsis construction; generalized boundary operator; added new explode option for post-processing views; enhanced link view behavior (to update only the changed items); added new default plugins: Skin, Transform, Smooth; fixed various other small bugs (mostly in the post-processing module and for extruded meshes). 1.22 (Aug 03, 2001): fixed (yet another) bug for 2D mesh in the mean plane; fixed surface coherence bug in extruded meshes; new double logarithmic scale, saturate value and smoothed normals option for post-processing views; plugins are now enabled by default; three new experimental statically linked plugins: CutMap (extracts a given iso surface from a 3D scalar map), CutPlane (cuts a 3D scalar map with a plane section), CutSphere (cuts a 3D scalar map with a sphere); various other bug fixes, additions and clean-ups. 1.21 (Jul 25, 2001): fixed more memory leaks; added -opt command line option to parse definitions directly from the command line; fixed missing screen refreshes during contour/surface/volume selection; enhanced string manipulation functions (Sprintf, StrCat, StrPrefix); many other small fixes and clean-ups. 1.20 (Jun 14, 2001): fixed various bugs (memory leaks, functions in included files, solver command selection, ColorTable option, duplicate nodes in extruded meshes (not finished yet), infinite loop on empty views, orientation of recombined quadrangles, ...); reorganized the interface menus; added constrained background mesh and mesh visibility options; added mesh quality histograms; changed default mesh colors; reintegrated the old command-line extrusion mesh generator. 1.19 (May 07, 2001): fixed seg. fault for scalar simplex post-processing; new Solver menu; interface for GetDP solver through sockets; fixed multiple scale alignment; added some options + full option descriptions. 1.18 (Apr 26, 2001): fixed many small bugs and incoherences in post-processing; fixed broken background mesh in 1D mesh generation. 1.17 (Apr 17, 2001): corrected physical points saving; fixed parsing of DOS files (carriage return problems); easier geometrical selections (cursor change); plugin manager; enhanced variable arrays (sublist selection and affectation); line loop check; New arrow display; reduced number of 'fatal' errors + better handling in interactive mode; fixed bug when opening meshes; enhanced File->Open behavior for meshes and post-processing views. 1.16 (Feb 26, 2001): added single/double buffer selection (only useful for Unix versions of Gmsh run from remote hosts without GLX); fixed a bug for recent versions of the opengl32.dll on Windows, which caused OpenGL fonts not to show up. 1.15 (Feb 23, 2001): added automatic visibility setting during entity selection; corrected geometrical extrusion bug. 1.14 (Feb 17, 2001): corrected a few bugs in the GUI (most of them were introduced in 1.13); added interactive color selection; made the option database bidirectional (i.e. scripts now correctly update the GUI); default options can now be saved and automatically reloaded at startup; made some changes to the scripting syntax (PostProcessing.View[n] becomes View[n]; Offset0 becomes OffsetX, etc.); corrected the handling of simple triangular surfaces with large characteristic lengths in the 2D isotropic algorithm; added an ASCII to binary post-processing view converter. 1.13 (Feb 09, 2001): added support for JPEG output on Windows. 1.12: corrected vector lines in the post-processing parsed format; corrected animation on Windows; corrected file creation in scripts on Windows; direct affectation of variable arrays. 1.11 (Feb 07, 2001): corrected included file loading problem. 1.10 (Feb 04, 2001): switched from Motif to FLTK for the GUI. Many small tweaks. 1.00 (Jan 15, 2001): added PPM and YUV output; corrected nested If/Endif; Corrected several bugs for pixel output and enhanced GIF output (dithering, transparency); slightly changed the post-processing file format to allow both single and double precision numbers. 0.999 (Dec 20, 2000): added JPEG output and easy MPEG generation (see t8.geo in the tutorial); clean up of export functions; small fixes; Linux versions are now compiled with gcc 2.95.2, which should fix the problems encountered with Mandrake 7.2. 0.998 (Dec 19, 2000): corrected bug introduced in 0.997 in the generation of the initial 3D mesh. 0.997 (Dec 14, 2000): corrected bug in interactive surface/volume selection; Added interactive symmetry; corrected geometrical extrusion with rotation in degenerated or partially degenerated cases; corrected bug in 2D mesh when meshing in the mean plane. 0.996: arrays of variables; enhanced Printf and Sprintf; Simplified options (suppression of option arrays). 0.995 (Dec 11, 2000): totally rewritten geometrical database (performance has been drastically improved for all geometrical transformations, and most notably for extrusion). As a consequence, the internal numbering of geometrical entities has changed: this will cause incompatibilities with old .geo files, and will require a partial rewrite of your old .geo files if these files made use of geometrical transformations. The syntax of the .geo file has also been clarified. Many additions for scripting purposes. New extrusion mesh generator. Preliminary version of the coupling between extruded and Delaunay meshes. New option and procedural database. All interactive operations can be scripted in the input files. See the last example in the tutorial for an example. Many stability enhancements in the 2D and 3D mesh algorithms. Performance boost of the 3D algorithm. Gmsh is still slow, but the performance becomes acceptable. An average 1000 tetrahedra/second is obtained on a 600Mhz computer for a mesh of one million tetrahedra. New anisotropic 2D mesh algorithm. New (ASCII and binary) post-processing file format and clarified mesh file format. New handling for interactive rotations (trackball mode). New didactic interactive mesh construction (watch the Delaunay algorithm in real time on complex geometries: that's exciting ;-). And many, many bug fixes and cleanups. 0.992 (Nov 13, 2000): corrected recombined extrusion; corrected ellipses; added simple automatic animation of post-processing maps; fixed various bugs. 0.991 (Oct 24, 2000): fixed a serious allocation bug in 2D algorithm, which caused random crashes. All users should upgrade to 0.991. 0.990: bug fix in non-recombined 3D transfinite meshes. 0.989 (Sep 01, 2000): added ability to reload previously saved meshes; some new command line options; reorganization of the scale menu; GIF output. 0.987: fixed bug with smoothing (leading to the possible generation of erroneous 3d meshes); corrected bug for mixed 3D meshes; moved the 'toggle view link' option to Opt->Postprocessing_Options. 0.986: fixed overlay problems; SGI version should now also run on 32 bits machines; fixed small 3d mesh bug. 0.985: corrected colormap bug on HP, SUN, SGI and IBM versions; corrected small initialization bug in postscript output. 0.984: corrected bug in display lists; added some options in Opt->General. 0.983: corrected some seg. faults in interactive mode; corrected bug in rotations; changed default window sizes for better match with 1024x768 screens (default X resources can be changed: see ex03.geo). 0.982: lighting for mesh and post-processing; corrected 2nd order mesh on non plane surfaces; added example 13.
Next: License, Previous: Version history, Up: Gmsh [Contents][Index]
Gmsh is copyright (C) 1997-2021 Christophe Geuzaine <cgeuzaine at uliege.be> and Jean-Francois Remacle <jean-francois.remacle at uclouvain.be> Code contributions to Gmsh have been provided by David Colignon (colormaps), Emilie Marchandise (old compound geometrical entities), Gaetan Bricteux (Gauss integration and levelsets), Jacques Lechelle (DIFFPACK export), Jonathan Lambrechts (mesh size fields, solver, Python wrappers), Jozef Vesely (old Tetgen integration), Koen Hillewaert (high order elements, generalized periodic meshes), Laurent Stainier (eigenvalue solvers, tensor display and help with MacOS port), Marc Ume (original list and tree code), Mark van Doesburg (old OpenCASCADE face connection), Matt Gundry (Plot3d export), Matti Pellikka (cell complex and homology solver), Nicolas Tardieu (help with Netgen integration), Pascale Noyret (MED mesh IO), Pierre Badel (root finding and minimization), Ruth Sabariego (pyramids), Stephen Guzik (old CGNS IO, old partitioning code), Bastien Gorissen (parallel remote post-processing), Eric Bechet (solver), Gilles Marckmann (camera and stero mode, X3D export), Ashish Negi (Netgen CAD healing), Trevor Strickler (hybrid structured mesh coupling with pyramids), Amaury Johnen (Bezier code, high-order element validity), Benjamin Ruard (old Java wrappers), Maxime Graulich (iOS/Android port), Francois Henrotte (ONELAB metamodels), Sebastian Eiser (PGF export), Alexis Salzman (compressed IO), Hang Si (TetGen/BR boundary recovery code), Fernando Lorenzo (Tochnog export), Larry Price (Gambit export), Anthony Royer (new partitioning code, MSH4 IO), Darcy Beurle (code cleanup and performance improvements), Celestin Marot (HXT/tetMesh), Pierre-Alexandre Beaufort (HXT/reparam), Zhidong Han (LSDYNA export), Ismail Badia (hierarchical basis functions), Jeremy Theler (X3D export), Thomas Toulorge (high order mesh optimizer, new CGNS IO), Max Orok (binary PLY), Marek Wojciechowski (PyPi packaging), Maxence Reberol (automatic transfinite), Michael Ermakov (Gambit export). See comments in the sources for more information. If we forgot to list your contributions please send us an email! Thanks to the following folks who have contributed by providing fresh ideas on theoretical or programming topics, who have sent patches, requests for changes or improvements, or who gave us access to exotic machines for testing Gmsh: Juan Abanto, Olivier Adam, Guillaume Alleon, Laurent Champaney, Pascal Dupuis, Patrick Dular, Philippe Geuzaine, Johan Gyselinck, Francois Henrotte, Benoit Meys, Nicolas Moes, Osamu Nakamura, Chad Schmutzer, Jean-Luc Fl'ejou, Xavier Dardenne, Christophe Prud'homme, Sebastien Clerc, Jose Miguel Pasini, Philippe Lussou, Jacques Kools, Bayram Yenikaya, Peter Hornby, Krishna Mohan Gundu, Christopher Stott, Timmy Schumacher, Carl Osterwisch, Bruno Frackowiak, Philip Kelleners, Romuald Conty, Renaud Sizaire, Michel Benhamou, Tom De Vuyst, Kris Van den Abeele, Simon Vun, Simon Corbin, Thomas De-Soza, Marcus Drosson, Antoine Dechaume, Jose Paulo Moitinho de Almeida, Thomas Pinchard, Corrado Chisari, Axel Hackbarth, Peter Wainwright, Jiri Hnidek, Thierry Thomas, Konstantinos Poulios, Laurent Van Miegroet, Shahrokh Ghavamian, Geordie McBain, Jose Paulo Moitinho de Almeida, Guillaume Demesy, Wendy Merks-Swolfs, Cosmin Stefan Deaconu, Nigel Nunn, Serban Georgescu, Julien Troufflard, Michele Mocciola, Matthijs Sypkens Smit, Sauli Ruuska, Romain Boman, Fredrik Ekre, Mark Burton, Max Orok, Paul Cristini, Isuru Fernando, Jose Paulo Moitinho de Almeida, Sophie Le Bras, Alberto Escrig, Samy Mukadi, Peter Johnston, Bruno de Sousa Alves, Stefan Bruens, Luca Verzeroli, Tristan Seidlhofer, Ding Jiaming, Joost Gevaert, Marcus Calhoun-Lopez, Michel Zou, Sir Sunsheep, Mariano Forti, Walter Steffe, Nico Schloemer, Simon Tournier, Alexandru Dadalau, Thomas Ulrich. Special thanks to Bill Spitzak, Michael Sweet, Matthias Melcher, Greg Ercolano and others for the Fast Light Tool Kit on which Gmsh's GUI is based. See http://www.fltk.org for more info on this excellent object-oriented, cross-platform toolkit. Special thanks also to EDF for funding the original OpenCASCADE and MED integration in 2006-2007. The TetGen/BR code (Mesh/tetgenBR.{cpp,h}) is copyright (c) 2016 Hang Si, Weierstrass Institute for Applied Analysis and Stochatics. It is relicensed under the terms of LICENSE.txt for use in Gmsh thanks to a Software License Agreement between Weierstrass Institute for Applied Analysis and Stochastics and GMESH SPRL. The AVL tree code (Common/avl.{cpp,h}) and the YUV image code (Graphics/gl2yuv.{cpp,h}) are copyright (C) 1988-1993, 1995 The Regents of the University of California. Permission to use, copy, modify, and distribute this software and its documentation for any purpose and without fee is hereby granted, provided that the above copyright notice appear in all copies and that both that copyright notice and this permission notice appear in supporting documentation, and that the name of the University of California not be used in advertising or publicity pertaining to distribution of the software without specific, written prior permission. The University of California makes no representations about the suitability of this software for any purpose. It is provided "as is" without express or implied warranty. The picojson code (Common/picojson.h) is Copyright 2009-2010 Cybozu Labs, Inc., Copyright 2011-2014 Kazuho Oku, All rights reserved. Redistribution and use in source and binary forms, with or without modification, are permitted provided that the following conditions are met: 1. Redistributions of source code must retain the above copyright notice, this list of conditions and the following disclaimer. 2. Redistributions in binary form must reproduce the above copyright notice, this list of conditions and the following disclaimer in the documentation and/or other materials provided with the distribution. THIS SOFTWARE IS PROVIDED BY THE COPYRIGHT HOLDERS AND CONTRIBUTORS "AS IS" AND ANY EXPRESS OR IMPLIED WARRANTIES, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE ARE DISCLAIMED. IN NO EVENT SHALL THE COPYRIGHT HOLDER OR CONTRIBUTORS BE LIABLE FOR ANY DIRECT, INDIRECT, INCIDENTAL, SPECIAL, EXEMPLARY, OR CONSEQUENTIAL DAMAGES (INCLUDING, BUT NOT LIMITED TO, PROCUREMENT OF SUBSTITUTE GOODS OR SERVICES; LOSS OF USE, DATA, OR PROFITS; OR BUSINESS INTERRUPTION) HOWEVER CAUSED AND ON ANY THEORY OF LIABILITY, WHETHER IN CONTRACT, STRICT LIABILITY, OR TORT (INCLUDING NEGLIGENCE OR OTHERWISE) ARISING IN ANY WAY OUT OF THE USE OF THIS SOFTWARE, EVEN IF ADVISED OF THE POSSIBILITY OF SUCH DAMAGE. The nanoflann code (Numeric/nanoflann.hpp) is Copyright 2008-2009 Marius Muja, 2008-2009 David G. Lowe, 2011-2016 Jose Luis Blanco. Redistribution and use in source and binary forms, with or without modification, are permitted provided that the following conditions are met: 1. Redistributions of source code must retain the above copyright notice, this list of conditions and the following disclaimer. 2. Redistributions in binary form must reproduce the above copyright notice, this list of conditions and the following disclaimer in the documentation and/or other materials provided with the distribution. THIS SOFTWARE IS PROVIDED BY THE AUTHOR ``AS IS'' AND ANY EXPRESS OR IMPLIED WARRANTIES, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE ARE DISCLAIMED. IN NO EVENT SHALL THE AUTHOR BE LIABLE FOR ANY DIRECT, INDIRECT, INCIDENTAL, SPECIAL, EXEMPLARY, OR CONSEQUENTIAL DAMAGES (INCLUDING, BUT NOT LIMITED TO, PROCUREMENT OF SUBSTITUTE GOODS OR SERVICES; LOSS OF USE, DATA, OR PROFITS; OR BUSINESS INTERRUPTION) HOWEVER CAUSED AND ON ANY THEORY OF LIABILITY, WHETHER IN CONTRACT, STRICT LIABILITY, OR TORT (INCLUDING NEGLIGENCE OR OTHERWISE) ARISING IN ANY WAY OUT OF THE USE OF THIS SOFTWARE, EVEN IF ADVISED OF THE POSSIBILITY OF SUCH DAMAGE. The trackball code (Graphics/Trackball.{cpp.h}) is copyright (C) 1993, 1994, Silicon Graphics, Inc. ALL RIGHTS RESERVED. Permission to use, copy, modify, and distribute this software for any purpose and without fee is hereby granted, provided that the above copyright notice appear in all copies and that both the copyright notice and this permission notice appear in supporting documentation, and that the name of Silicon Graphics, Inc. not be used in advertising or publicity pertaining to distribution of the software without specific, written prior permission. The GIF and PPM routines (Graphics/gl2gif.cpp) are based on code copyright (C) 1989, 1991, Jef Poskanzer. Permission to use, copy, modify, and distribute this software and its documentation for any purpose and without fee is hereby granted, provided that the above copyright notice appear in all copies and that both that copyright notice and this permission notice appear in supporting documentation. This software is provided "as is" without express or implied warranty. The colorbar widget (Fltk/colorbarWindow.cpp) was inspired by code from the Vis5d program for visualizing five dimensional gridded data sets, copyright (C) 1990-1995, Bill Hibbard, Brian Paul, Dave Santek, and Andre Battaiola. In addition, this version of Gmsh may contain the following contributed, optional codes in the contrib/ directory, each governed by their own license: * contrib/ANN copyright (C) 1997-2005 University of Maryland and Sunil Arya and David Mount; * contrib/gmm copyright (C) 2002-2008 Yves Renard; * contrib/hxt - Copyright (C) 2017-2018 - Universite catholique de Louvain; * contrib/kbipack copyright (C) 2005 Saku Suuriniemi; * contrib/MathEx based in part on the work of the SSCILIB Library, copyright (C) 2000-2003 Sadao Massago; * contrib/metis written by George Karypis (karypis at cs.umn.edu), copyright (C) 1995-2013 Regents of the University of Minnesota; * contrib/mpeg_encode copyright (c) 1995 The Regents of the University of California; * contrib/Netgen copyright (C) 1994-2004 Joachim Sch"oberl; * contrib/bamg from Freefem++ copyright (C) Frederic Hecht; * contrib/ALGLIB (C) Sergey Bochkanov (ALGLIB project); * contrib/blossom copyright (C) 1995-1997 Bill Cook et al.; * contrib/bamg from Freefem++ copyright (C) Frederic Hecht; * contrib/voro++ from Voro++ Copyright (c) 2008, The Regents of the University of California, through Lawrence Berkeley National Laboratory (subject to receipt of any required approvals from the U.S. Dept. of Energy). All rights reserved; * contrib/zipper from MiniZip - Copyright (c) 1998-2010 - by Gilles Vollant - version 1.1 64 bits from Mathias Svensson. heck the configuration options to see which have been enabled.
Next: Concept index, Previous: Copyright and credits, Up: Gmsh [Contents][Index]
Gmsh is provided under the terms of the GNU General Public License (GPL), Version 2 or later, with the following exception: The copyright holders of Gmsh give you permission to combine Gmsh with code included in the standard release of Netgen (from Joachim Sch"oberl), METIS (from George Karypis at the University of Minnesota), OpenCASCADE (from Open CASCADE S.A.S) and ParaView (from Kitware, Inc.) under their respective licenses. You may copy and distribute such a system following the terms of the GNU GPL for Gmsh and the licenses of the other code concerned, provided that you include the source code of that other code when and as the GNU GPL requires distribution of source code. Note that people who make modified versions of Gmsh are not obligated to grant this special exception for their modified versions; it is their choice whether to do so. The GNU General Public License gives permission to release a modified version without this exception; this exception also makes it possible to release a modified version which carries forward this exception. End of exception. GNU GENERAL PUBLIC LICENSE Version 2, June 1991 Copyright (C) 1989, 1991 Free Software Foundation, Inc. 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA Everyone is permitted to copy and distribute verbatim copies of this license document, but changing it is not allowed. Preamble The licenses for most software are designed to take away your freedom to share and change it. By contrast, the GNU General Public License is intended to guarantee your freedom to share and change free software--to make sure the software is free for all its users. This General Public License applies to most of the Free Software Foundation's software and to any other program whose authors commit to using it. (Some other Free Software Foundation software is covered by the GNU Library General Public License instead.) You can apply it to your programs, too. When we speak of free software, we are referring to freedom, not price. Our General Public Licenses are designed to make sure that you have the freedom to distribute copies of free software (and charge for this service if you wish), that you receive source code or can get it if you want it, that you can change the software or use pieces of it in new free programs; and that you know you can do these things. To protect your rights, we need to make restrictions that forbid anyone to deny you these rights or to ask you to surrender the rights. These restrictions translate to certain responsibilities for you if you distribute copies of the software, or if you modify it. For example, if you distribute copies of such a program, whether gratis or for a fee, you must give the recipients all the rights that you have. You must make sure that they, too, receive or can get the source code. And you must show them these terms so they know their rights. We protect your rights with two steps: (1) copyright the software, and (2) offer you this license which gives you legal permission to copy, distribute and/or modify the software. Also, for each author's protection and ours, we want to make certain that everyone understands that there is no warranty for this free software. If the software is modified by someone else and passed on, we want its recipients to know that what they have is not the original, so that any problems introduced by others will not reflect on the original authors' reputations. Finally, any free program is threatened constantly by software patents. We wish to avoid the danger that redistributors of a free program will individually obtain patent licenses, in effect making the program proprietary. To prevent this, we have made it clear that any patent must be licensed for everyone's free use or not licensed at all. The precise terms and conditions for copying, distribution and modification follow. GNU GENERAL PUBLIC LICENSE TERMS AND CONDITIONS FOR COPYING, DISTRIBUTION AND MODIFICATION 0. This License applies to any program or other work which contains a notice placed by the copyright holder saying it may be distributed under the terms of this General Public License. The "Program", below, refers to any such program or work, and a "work based on the Program" means either the Program or any derivative work under copyright law: that is to say, a work containing the Program or a portion of it, either verbatim or with modifications and/or translated into another language. (Hereinafter, translation is included without limitation in the term "modification".) Each licensee is addressed as "you". Activities other than copying, distribution and modification are not covered by this License; they are outside its scope. The act of running the Program is not restricted, and the output from the Program is covered only if its contents constitute a work based on the Program (independent of having been made by running the Program). Whether that is true depends on what the Program does. 1. You may copy and distribute verbatim copies of the Program's source code as you receive it, in any medium, provided that you conspicuously and appropriately publish on each copy an appropriate copyright notice and disclaimer of warranty; keep intact all the notices that refer to this License and to the absence of any warranty; and give any other recipients of the Program a copy of this License along with the Program. You may charge a fee for the physical act of transferring a copy, and you may at your option offer warranty protection in exchange for a fee. 2. You may modify your copy or copies of the Program or any portion of it, thus forming a work based on the Program, and copy and distribute such modifications or work under the terms of Section 1 above, provided that you also meet all of these conditions: a) You must cause the modified files to carry prominent notices stating that you changed the files and the date of any change. b) You must cause any work that you distribute or publish, that in whole or in part contains or is derived from the Program or any part thereof, to be licensed as a whole at no charge to all third parties under the terms of this License. c) If the modified program normally reads commands interactively when run, you must cause it, when started running for such interactive use in the most ordinary way, to print or display an announcement including an appropriate copyright notice and a notice that there is no warranty (or else, saying that you provide a warranty) and that users may redistribute the program under these conditions, and telling the user how to view a copy of this License. (Exception: if the Program itself is interactive but does not normally print such an announcement, your work based on the Program is not required to print an announcement.) These requirements apply to the modified work as a whole. If identifiable sections of that work are not derived from the Program, and can be reasonably considered independent and separate works in themselves, then this License, and its terms, do not apply to those sections when you distribute them as separate works. But when you distribute the same sections as part of a whole which is a work based on the Program, the distribution of the whole must be on the terms of this License, whose permissions for other licensees extend to the entire whole, and thus to each and every part regardless of who wrote it. Thus, it is not the intent of this section to claim rights or contest your rights to work written entirely by you; rather, the intent is to exercise the right to control the distribution of derivative or collective works based on the Program. In addition, mere aggregation of another work not based on the Program with the Program (or with a work based on the Program) on a volume of a storage or distribution medium does not bring the other work under the scope of this License. 3. You may copy and distribute the Program (or a work based on it, under Section 2) in object code or executable form under the terms of Sections 1 and 2 above provided that you also do one of the following: a) Accompany it with the complete corresponding machine-readable source code, which must be distributed under the terms of Sections 1 and 2 above on a medium customarily used for software interchange; or, b) Accompany it with a written offer, valid for at least three years, to give any third party, for a charge no more than your cost of physically performing source distribution, a complete machine-readable copy of the corresponding source code, to be distributed under the terms of Sections 1 and 2 above on a medium customarily used for software interchange; or, c) Accompany it with the information you received as to the offer to distribute corresponding source code. (This alternative is allowed only for noncommercial distribution and only if you received the program in object code or executable form with such an offer, in accord with Subsection b above.) The source code for a work means the preferred form of the work for making modifications to it. For an executable work, complete source code means all the source code for all modules it contains, plus any associated interface definition files, plus the scripts used to control compilation and installation of the executable. However, as a special exception, the source code distributed need not include anything that is normally distributed (in either source or binary form) with the major components (compiler, kernel, and so on) of the operating system on which the executable runs, unless that component itself accompanies the executable. If distribution of executable or object code is made by offering access to copy from a designated place, then offering equivalent access to copy the source code from the same place counts as distribution of the source code, even though third parties are not compelled to copy the source along with the object code. 4. You may not copy, modify, sublicense, or distribute the Program except as expressly provided under this License. Any attempt otherwise to copy, modify, sublicense or distribute the Program is void, and will automatically terminate your rights under this License. However, parties who have received copies, or rights, from you under this License will not have their licenses terminated so long as such parties remain in full compliance. 5. You are not required to accept this License, since you have not signed it. However, nothing else grants you permission to modify or distribute the Program or its derivative works. These actions are prohibited by law if you do not accept this License. Therefore, by modifying or distributing the Program (or any work based on the Program), you indicate your acceptance of this License to do so, and all its terms and conditions for copying, distributing or modifying the Program or works based on it. 6. Each time you redistribute the Program (or any work based on the Program), the recipient automatically receives a license from the original licensor to copy, distribute or modify the Program subject to these terms and conditions. You may not impose any further restrictions on the recipients' exercise of the rights granted herein. You are not responsible for enforcing compliance by third parties to this License. 7. If, as a consequence of a court judgment or allegation of patent infringement or for any other reason (not limited to patent issues), conditions are imposed on you (whether by court order, agreement or otherwise) that contradict the conditions of this License, they do not excuse you from the conditions of this License. If you cannot distribute so as to satisfy simultaneously your obligations under this License and any other pertinent obligations, then as a consequence you may not distribute the Program at all. For example, if a patent license would not permit royalty-free redistribution of the Program by all those who receive copies directly or indirectly through you, then the only way you could satisfy both it and this License would be to refrain entirely from distribution of the Program. If any portion of this section is held invalid or unenforceable under any particular circumstance, the balance of the section is intended to apply and the section as a whole is intended to apply in other circumstances. It is not the purpose of this section to induce you to infringe any patents or other property right claims or to contest validity of any such claims; this section has the sole purpose of protecting the integrity of the free software distribution system, which is implemented by public license practices. Many people have made generous contributions to the wide range of software distributed through that system in reliance on consistent application of that system; it is up to the author/donor to decide if he or she is willing to distribute software through any other system and a licensee cannot impose that choice. This section is intended to make thoroughly clear what is believed to be a consequence of the rest of this License. 8. If the distribution and/or use of the Program is restricted in certain countries either by patents or by copyrighted interfaces, the original copyright holder who places the Program under this License may add an explicit geographical distribution limitation excluding those countries, so that distribution is permitted only in or among countries not thus excluded. In such case, this License incorporates the limitation as if written in the body of this License. 9. The Free Software Foundation may publish revised and/or new versions of the General Public License from time to time. Such new versions will be similar in spirit to the present version, but may differ in detail to address new problems or concerns. Each version is given a distinguishing version number. If the Program specifies a version number of this License which applies to it and "any later version", you have the option of following the terms and conditions either of that version or of any later version published by the Free Software Foundation. If the Program does not specify a version number of this License, you may choose any version ever published by the Free Software Foundation. 10. If you wish to incorporate parts of the Program into other free programs whose distribution conditions are different, write to the author to ask for permission. For software which is copyrighted by the Free Software Foundation, write to the Free Software Foundation; we sometimes make exceptions for this. Our decision will be guided by the two goals of preserving the free status of all derivatives of our free software and of promoting the sharing and reuse of software generally. NO WARRANTY 11. BECAUSE THE PROGRAM IS LICENSED FREE OF CHARGE, THERE IS NO WARRANTY FOR THE PROGRAM, TO THE EXTENT PERMITTED BY APPLICABLE LAW. EXCEPT WHEN OTHERWISE STATED IN WRITING THE COPYRIGHT HOLDERS AND/OR OTHER PARTIES PROVIDE THE PROGRAM "AS IS" WITHOUT WARRANTY OF ANY KIND, EITHER EXPRESSED OR IMPLIED, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE. THE ENTIRE RISK AS TO THE QUALITY AND PERFORMANCE OF THE PROGRAM IS WITH YOU. SHOULD THE PROGRAM PROVE DEFECTIVE, YOU ASSUME THE COST OF ALL NECESSARY SERVICING, REPAIR OR CORRECTION. 12. IN NO EVENT UNLESS REQUIRED BY APPLICABLE LAW OR AGREED TO IN WRITING WILL ANY COPYRIGHT HOLDER, OR ANY OTHER PARTY WHO MAY MODIFY AND/OR REDISTRIBUTE THE PROGRAM AS PERMITTED ABOVE, BE LIABLE TO YOU FOR DAMAGES, INCLUDING ANY GENERAL, SPECIAL, INCIDENTAL OR CONSEQUENTIAL DAMAGES ARISING OUT OF THE USE OR INABILITY TO USE THE PROGRAM (INCLUDING BUT NOT LIMITED TO LOSS OF DATA OR DATA BEING RENDERED INACCURATE OR LOSSES SUSTAINED BY YOU OR THIRD PARTIES OR A FAILURE OF THE PROGRAM TO OPERATE WITH ANY OTHER PROGRAMS), EVEN IF SUCH HOLDER OR OTHER PARTY HAS BEEN ADVISED OF THE POSSIBILITY OF SUCH DAMAGES. END OF TERMS AND CONDITIONS How to Apply These Terms to Your New Programs If you develop a new program, and you want it to be of the greatest possible use to the public, the best way to achieve this is to make it free software which everyone can redistribute and change under these terms. To do so, attach the following notices to the program. It is safest to attach them to the start of each source file to most effectively convey the exclusion of warranty; and each file should have at least the "copyright" line and a pointer to where the full notice is found. <one line to give the program's name and a brief idea of what it does.> Copyright (C) <year> <name of author> This program is free software; you can redistribute it and/or modify it under the terms of the GNU General Public License as published by the Free Software Foundation; either version 2 of the License, or (at your option) any later version. This program is distributed in the hope that it will be useful, but WITHOUT ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License for more details. You should have received a copy of the GNU General Public License along with this program; if not, write to the Free Software Foundation, Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 USA Also add information on how to contact you by electronic and paper mail. If the program is interactive, make it output a short notice like this when it starts in an interactive mode: Gnomovision version 69, Copyright (C) year name of author Gnomovision comes with ABSOLUTELY NO WARRANTY; for details type `show w'. This is free software, and you are welcome to redistribute it under certain conditions; type `show c' for details. The hypothetical commands `show w' and `show c' should show the appropriate parts of the General Public License. Of course, the commands you use may be called something other than `show w' and `show c'; they could even be mouse-clicks or menu items--whatever suits your program. You should also get your employer (if you work as a programmer) or your school, if any, to sign a "copyright disclaimer" for the program, if necessary. Here is a sample; alter the names: Yoyodyne, Inc., hereby disclaims all copyright interest in the program `Gnomovision' (which makes passes at compilers) written by James Hacker. <signature of Ty Coon>, 1 April 1989 Ty Coon, President of Vice This General Public License does not permit incorporating your program into proprietary programs. If your program is a subroutine library, you may consider it more useful to permit linking proprietary applications with the library. If this is what you want to do, use the GNU Library General Public License instead of this License.
Next: Syntax index, Previous: License, Up: Gmsh [Contents][Index]
Jump to: | 2
3
A B C D E F G H I K L M N O P Q R S T U V W |
---|
Jump to: | 2
3
A B C D E F G H I K L M N O P Q R S T U V W |
---|
Previous: Concept index, Up: Gmsh [Contents][Index]
Jump to: | !
%
&
(
*
+
-
/
:
<
=
>
?
^
|
A B C D E F G H I L M N O P R S T U V W |
---|
Jump to: | !
%
&
(
*
+
-
/
:
<
=
>
?
^
|
A B C D E F G H I L M N O P R S T U V W |
---|
Nearly all the interactive commands have keyboard shortcuts: see Keyboard shortcuts, or select ‘Help->Keyboard and Mouse Usage’ in the menu. For example, to quickly save a mesh, you can press Ctrl+Shift+s.
If you compile Gmsh without the GUI (see Compiling the source code), this is the only mode you have access to.
The affectation operators are introduced in General commands.
For
compatibility purposes, the behavior of newl
, news
,
newv
and newreg
can be modified with the
Geometry.OldNewReg
option (see Geometry options list).
R. A. Dwyer, A simple divide-and-conquer algorithm for computing Delaunay triangulations in O(n log n) expected time, In Proceedings of the second annual symposium on computational geometry, Yorktown Heights, 2–4 June 1986.
N. P. Weatherill, The integrity of geometrical boundaries in the two-dimensional Delaunay triangulation, Commun. Appl. Numer. Methods 6(2), pp. 101–109, 1990.
C. Geuzaine and J.-F. Remacle, Gmsh: a three-dimensional finite element mesh generator with built-in pre- and post-processing facilities, International Journal for Numerical Methods in Engineering 79(11), pp. 1309–1331, 2009.
P.-L. George and P. Frey, Mesh generation, Hermes, Lyon, 2000.
S. Rebay, Efficient unstructured mesh generation by means of Delaunay triangulation and Bowyer-Watson algorithm, J. Comput. Phys. 106, pp. 25–138, 1993.
J.-F. Remacle, F. Henrotte, T. Carrier-Baudouin, E. Béchet, E. Marchandise, C. Geuzaine and T. Mouton, A frontal Delaunay quad mesh generator using the Linf norm, International Journal for Numerical Methods in Engineering, 94(5), pp. 494-512, 2013.
F. Hecht, BAMG: bidimensional anisotropic mesh generator, User Guide, INRIA, Rocquencourt, 1998.
J. Schoeberl, Netgen, an advancing front 2d/3d-mesh generator based on abstract rules, Comput. Visual. Sci., 1, pp. 41–52, 1997.
C. Marot, J. Pellerin and J.‐F. Remacle, One machine, one minute, three billion tetrahedra, International Journal for Numerical Methods in Engineering 117.9, pp 967-990, 2019.
C. Dobrzynski, MMG3D: user guide, INRIA, 2012.
If the numbering is not too sparse, Gmsh will still use a vector.
Each step can be linked to a different model, which allows to have a single time series based on multiple (e.g. deforming or moving) meshes.