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-basedx5
: Additional geometrical data: parametrizations, normals, curvaturesx6
: Additional mesh data: integration points, Jacobians and basis functionsx7
: Additional mesh data: internal edges and facesgmsh
: 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/view/option
: view option handling functionsgmsh/plugin
: plugin functionsgmsh/graphics
: graphics functionsgmsh/fltk
: FLTK graphical user interface functionsgmsh/parser
: parser functionsgmsh/onelab
: ONELAB server functionsgmsh/logger
: information logging functionsNext: 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 4.10.2 (May 13, 2022).
• Obtaining Gmsh | Where to get your copy of Gmsh | |
• Copying conditions | Terms and conditions of use | |
• Overview | What is Gmsh? | |
• How to read this manual? | Which parts of this manual should you read (if any)? | |
• Running Gmsh on your system | How can you run Gmsh on your machine? | |
• General tools | Description of general commands and options | |
• Geometry module | Description of all Geometry commands | |
• Mesh module | Description of all Mesh commands | |
• Solver module | Description of all Solver commands | |
• Post-processing module | Description of all Post-Processing commands | |
• File formats | Input and output file formats | |
• Tutorial | A step-by-step tutorial | |
• Options | List of all available options | |
• Compiling the source code | Information on how to comile Gmsh from source | |
• Gmsh API | Gmsh Application Programming Interface | |
• Information for developers | Information for Gmsh developers | |
• Frequently asked questions | The Gmsh FAQ | |
• Version history | Changelog | |
• Copyright and credits | Copyright information and list of contributors | |
• License | Complete copy of the license | |
• Concept index | Index of concepts | |
• Syntax index | Index of command line, scripting and API syntax |
Next: Copying conditions, Previous: Top, Up: Top [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: Top [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 manual?, Previous: Copying conditions, Up: Top [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.
• Geometry | ||
• Mesh | ||
• Solver | ||
• Post-processing | ||
• What Gmsh is pretty good at | ||
• and what Gmsh is not so good at | ||
• Bug reports |
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.
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, Previous: Mesh, Up: Overview [Contents][Index]
Gmsh implements a ONELAB (http://onelab.info) server to exchange data with 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 examples/api. See in particular prepro.py, custom_gui.py and custom_gui.cpp.
Next: What Gmsh is pretty good at, Previous: Solver, 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, Up: Overview [Contents][Index]
Here is a tentative list of what Gmsh does best:
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: Top [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.
• Syntactic rules |
Previous: How to read this manual?, Up: How to read this 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 manual?, Up: Top [Contents][Index]
• Interactive mode | ||
• Non-interactive mode | ||
• Command-line options | ||
• Mouse actions | ||
• Keyboard shortcuts |
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, 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
-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, off (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, quadqs, 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
-save
Save output file, then exit
-o file
Specify output file name
-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, ONELAB or option number name=value
-setstring name value
Set constant, ONELAB 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
Toggle x coordinate freeze in geometry creation mode
Toggle y coordinate freeze in geometry creation mode
Toggle 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: Top [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.
• Comments | ||
• Expressions | ||
• Operators | ||
• Built-in functions | ||
• User-defined macros | ||
• Loops and conditionals | ||
• General commands | ||
• General options |
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.
• Floating point expressions | ||
• Character expressions | ||
• Color expressions |
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), 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, 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
src/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, 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:
-
Unary minus.
!
Logical not.
operator-unary-right:
++
Post-incrementation.
--
Post-decrementation.
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
Begin 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
End the body of the current user-defined macro. Macro declarations cannot be imbricated.
Call string | char-expression ;
Execute the body of a (previously defined) macro named string.
See t5, 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 )
Iterate 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 )
Iterate 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 }
Iterate 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 }
Iterate 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
End 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
End 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;
Create 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
Return 3.1415926535897932.
GMSH_MAJOR_VERSION
Return Gmsh’s major version number.
GMSH_MINOR_VERSION
Return Gmsh’s minor version number.
GMSH_PATCH_VERSION
Return Gmsh’s patch version number.
MPI_Size
Return 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
Return the rank of the current processor.
Cpu
Return the current CPU time (in seconds).
Memory
Return the current memory usage (in Mb).
TotalMemory
Return the total memory available (in Mb).
newp
Return 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.
newc
Return the next available curve tag.
news
Return the next available surface tag.
newv
Return the next available volume tag.
newcl
Return the next available curve loop tag.
newsl
Return the next available surface loop tag.
newreg
Return the next available region tag. That is, newreg
returns
the maximum of newp
, newl
, news
, newv
,
newll
, newsl
and all physical group tags4.
string = { };
Create a new expression list identifier string
with an
empty list.
string[] = { expression-list };
Create 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 };
Affect 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;
Add and affect expression to an existing expression identifier.
string -= expression;
Subtract and affect expression to an existing expression identifier.
string *= expression;
Multiply and affect expression to an existing expression identifier.
string /= expression;
Divide and affect expression to an existing expression identifier.
string += { expression-list };
Append expression-list to an existing expression list or creates a new expression list with expression-list.
string -= { expression-list };
Remove the items in expression-list from the existing expression list.
string [ { expression-list } ] += { expression-list };
Add and affect, 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 };
Subtract and affect, 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 };
Multiply and affect, 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 };
Divide and affect, 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;
Create a new character expression identifier string
with a
given char-expression.
string[] = Str( char-expression-list ) ;
Create 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 ) ;
Append a character expression list to an existing list. Parentheses can also be used instead of brackets.
DefineConstant[ string = expression|char-expression <, ...>];
Create 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 );
Set the value a numeric ONELAB variable char-expression.
SetString( char-expression , char-expression );
Set the value a string ONELAB variable char-expression.
real-option = expression;
Affect expression to a real option.
char-option = char-expression;
Affect char-expression to a character option.
color-option = color-expression;
Affect color-expression to a color option.
real-option += expression;
Add and affect expression to a real option.
real-option -= expression;
Subtract and affect expression to a real option.
real-option *= expression;
Multiply and affect expression to a real option.
real-option /= expression;
Divide and affect expression to a real option.
Abort;
Abort the current script.
Exit;
Exit Gmsh.
CreateDir char-expression;
Create the directory char-expression.
Printf ( char-expression <, expression-list> );
Print 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, 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;
Merge 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 );
Merge a BREP, STEP or IGES file and returns the tags of the highest-dimensional entities. Only available with the OpenCASCADE geometry kernel.
Draw;
Redraw the scene.
SplitCurrentWindowHorizontal expression;
Split the current window horizontally, with the ratio given by expression.
SplitCurrentWindowVertical expression;
Split the current window vertically, with the ratio given by expression.
SetCurrentWindow expression;
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.
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;
Recompute 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 };
Force 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;
Delete the current model (all model entities and their associated meshes).
Delete Physicals;
Delete all physical groups.
Delete Variables;
Delete all the expressions.
Delete Options;
Delete the current options and revert to the default values.
Delete string;
Delete the expression string.
Print char-expression;
Print 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;
Suspend the execution of Gmsh during expression seconds.
SystemCall char-expression;
Executes a (blocking) system call.
NonBlockingSystemCall char-expression;
Execute a (non-blocking) system call.
OnelabRun ( char-expression <, char-expression > )
Run a ONELAB client (first argument is the client name, second optional arguement is the command line).
SetName char-expression;
Change the name of the current model.
SetFactory(char-expression);
Change 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;
Force an immediate transfer from the old geometrical database into the new one (this transfer normally occurs right after a file is read).
NewModel;
Create a new current model.
Include char-expression;
Include 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: Top [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.
• Geometry commands | ||
• Geometry options |
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.”
• Points | ||
• Curves | ||
• Surfaces | ||
• Volumes | ||
• Extrusions | ||
• Boolean operations | ||
• Transformations | ||
• Miscellaneous geometry commands |
Next: Curves, Previous: Geometry commands, Up: Geometry commands [Contents][Index]
Point ( expression ) = { expression, expression, expression <, expression > };
Create 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 };
Create 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 };
Create 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 };
Create a Bezier curve. The expression-list contains the tags of the control points.
BSpline ( expression ) = { expression-list };
Create 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 };
Create 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 <, ...> };
Create a circle arc. If three expressions are provided on the right-hand-side they 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, if between 4 and 6 expressions are provided, the first three define the coordinates of the center, the next one defines the radius, and the optional next two the start and end angle.
Ellipse ( expression ) = { expression, expression, expression <, ...> };
Create 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;
Create 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 };
Create 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. With the built-in geometry kernel, 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; the built-in kernel also supports multiple curve loops (or
subloops) in a single Curve Loop
command, but this is not
recommended). With the OpenCASCADE kernel the curve loop is always
oriented according to the orientation of its first curve; negative tags
can be specified for compatibility with the built-in kernel, but are
simply ignored. Curve loops are used to create surfaces: see
Surfaces.
Wire ( expression ) = { expression-list };
Create 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 };
Create 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 };
Create 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 }, Using Point { expression-list } >;
Create a surface filling. With the built-in kernel, the first curve
loop should be composed of either three or four curves, the surface is
constructed using transfinite interpolation, and 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). With the
OpenCASCADE kernel, a BSpline surface is constructucted by optimization
to match the bounding curves, as well as the (optional) points provided
after Using Point
.
BSpline Surface ( expression ) = { expression-list };
Create 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 };
Create 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 };
Create 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 >;
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 };
Create 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 }
Extrude 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 }
Extrude 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 }
Extrude 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 }
Extrude 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 }
Extrude entities in extrude-list along the give wire. Only available with the OpenCASCADE geometry kernel.
ThruSections { expression-list }
Create surfaces through the given curve loops or
wires. ThruSections
is only available with the OpenCASCADE
kernel.
Ruled ThruSections { expression-list }
Create 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 }
Fillet 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 }
Compute the intersection of the object and the tool.
BooleanUnion { boolean-list } { boolean-list }
Compute the union of the object and the tool.
BooleanDifference { boolean-list } { boolean-list }
Subtract the tool from the object.
BooleanFragments { boolean-list } { boolean-list }
Compute 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 examples/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 };
Compute the intersection of the object and the tool and assign the result the tag expression.
BooleanUnion ( expression ) = { boolean-list } { boolean-list };
Compute 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 examples/boolean for examples.
Boolean operations are only available with the OpenCASCADE geometry kernel.
Next: Miscellaneous geometry commands, 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 }
Scale 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 }
Scale 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 }
Rotate 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 }
Transform 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 }
Apply 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 }
Translate 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.) Return 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.) Return 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.) Return 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.) Return 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.) Split the curve expression on the specified control points. Only available with the built-in kernel, for lines, splines and BSplines.
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;
Remove 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 geometry kernel,
Coherence
is simply a shortcut for a BooleanFragments
operation on all entities, with the Delete
operator applied to
all operands.
HealShapes;
Apply the shape healing procedure(s), according to
Geometry.OCCFixDegenerated
, Geometry.OCCFixSmallEdges
,
Geometry.OCCFixSmallFaces
, Geometry.OCCSewFaces
,
Geometry.OCCMakeSolids
. Only available with the OpenCASCADE
geometry kernel.
< Recursive > Delete { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
Delete 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 }; … }
Delete 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 )
Force 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.
Hide { : }
Hide all entities.
< Recursive > Show { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
Show the entities listed in expression-list-or-all.
Show { : }
Show all entities.
Sphere | PolarSphere ( expression ) = {expression, expression};
Change the current (surface) geometry used by the built-in geometry kernel to a (polar) sphere, defined by the two point tags specified on the right hand side. The expression between parentheses on the left hand side specifies a new unique tag for this geometry.
Parametric Surface ( expression ) = "string" "string" "string";
Change the current (surface) geometry used by the built-in geometry kernel to a parametric surface defined by the three strings expression evaluating to the x, y and z coordinates. The expression between parentheses on the left hand side specifies a new unique tag for this geometry.
Coordinates Surface expression;
Change the current (surface) geometry used by the built-in geometry kernel to the geometry identified by the given expression.
Euclidian Coordinates ;
Restore the default planar geometry for the built-in geometry kernel.
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: Top [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):
Recombine
commands (see Structured grids, and
Miscellaneous mesh commands). 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.SubdivisionAlgorithm
option
(see Mesh options list).
• Choosing the right unstructured algorithm | ||
• Elementary entities vs physical groups | ||
• Mesh commands | ||
• Mesh options |
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).
• Specifying mesh element sizes | ||
• Structured grids | ||
• Miscellaneous mesh commands |
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.
All the aforementioned methods can be used simultaneously, in which case
the smallest element size is selected at any given point. Using the
Gmsh API, the resulting value can be further modified using a C++, C,
Python or Julia mesh size callback function provided via
gmsh/model/mesh/setSizeCallback
(see Namespace gmsh/model/mesh). In addition, boundary mesh sizes are interpolated
inside surfaces and/or volumes depending on the value of
Mesh.MeshSizeExtendFromBoundary
.
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:
AttractorAnisoCurve
Compute the distance to the given curves and specify the mesh size independently in the direction normal and parallel to the nearest curve. For efficiency each curve is replaced by a set of Sampling 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
Sampling
Number of sampling points on 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
Return VIn inside a spherical ball, and 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: 1e+22
VOut
Value outside the ball
type: float
default value: 1e+22
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 constructed
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
Mesh 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
Return VIn inside the box, and VOut outside. 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: 1e+22
VOut
Value outside the box
type: float
default value: 1e+22
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
Constant
Return VIn when inside the entities (and on their boundary if IncludeBoundary is set), and VOut outside.
Options:
CurvesList
Curve tags
type: list
default value: {}
IncludeBoundary
Include the boundary of the entities
type: boolean
default value: 1
PointsList
Point tags
type: list
default value: {}
SurfacesList
Surface tags
type: list
default value: {}
VIn
Value inside the entities
type: float
default value: 1e+22
VOut
Value outside the entities
type: float
default value: 1e+22
VolumesList
Volume tags
type: list
default value: {}
Curvature
Compute the curvature of Field[InField]:
F = div(norm(grad(Field[InField])))
Options:
Delta
Step of the finite differences
type: float
default value: 0.0003464101615137755
InField
Input field tag
type: integer
default value: 1
Cylinder
Return VIn inside a frustrated cylinder, and VOut outside. The cylinder is defined 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: 1e+22
VOut
Value outside the cylinder
type: float
default value: 1e+22
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. For efficiency, curves and surfaces are replaced by a set of points (sampled according to Sampling), to which the distance is actually computed.
Options:
CurvesList
Tags of curves in the geometric model
type: list
default value: {}
PointsList
Tags of points in the geometric model
type: list
default value: {}
Sampling
Linear (i.e. per dimension) number of sampling points to discretize each curve and surface
type: integer
default value: 20
SurfacesList
Tags of surfaces in the geometric model (only OpenCASCADE and discrete surfaces are currently supported)
type: list
default value: {}
Extend
Compute an extension of the mesh sizes from the given boundary curves (resp. surfaces) inside the surfaces (resp. volumes) being meshed. If the mesh size on the boundary, computed as the local average length of the edges of the boundary elements, is denoted by SizeBnd, the extension is computed as:
F = f * SizeBnd + (1 - f) * SizeMax, if d < DistMax
F = SizeMax, if d >= DistMax
where d denotes the distance to the boundary and f = ((DistMax - d) / DistMax)^Power.
Options:
CurvesList
Tags of curves in the geometric model
type: list
default value: {}
DistMax
Maximum distance of the size extension
type: float
default value: 1
Power
Power exponent used to interpolate the mesh size
type: float
default value: 1
SizeMax
Mesh size outside DistMax
type: float
default value: 1
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
Interpolate mesh sizes on a extended cylinder frustrum defined by inner (R1i and R2i) and outer (R1o and R2o) radii and two endpoints P1 and P2.The field value F for a point P is 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)
F = (1 - v) * ((1 - u) * v1i + u * v2i) + v * ((1 - u) * v1o + u * v2o)
with (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
Mesh size at point 1, inner radius
type: float
default value: 0.1
InnerV2
Mesh 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
Mesh size at point 1, outer radius
type: float
default value: 1
OuterV2
Mesh 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: 0.0003464101615137755
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: 3
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: 0.0003464101615137755
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: 0.0003464101615137755
InField
Input field tag
type: integer
default value: 1
Mean
Return the mean value
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: 1
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: 1
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 with index ViewIndex, or with tag ViewTag if ViewTag is positive.
Options:
CropNegativeValues
return MAX_LC instead of a negative value (this option is needed for backward compatibility with the BackgroundMesh option
type: boolean
default value: 1
UseClosest
Use value at closest node if no exact match is found
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 (as well as their boundaries if IncludeBoundary is set).
Options:
CurvesList
Curve tags
type: list
default value: {}
InField
Input field tag
type: integer
default value: 1
IncludeBoundary
Include the boundary of the entities
type: boolean
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: 1e+22
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
Return F = SizeMin if Field[InField] <= DistMin, F = SizeMax if Field[InField] >= DistMax, and the interpolation between SizeMin and SizeMax if DistMin < Field[InField] < DistMax.
Options:
DistMax
Value after which the mesh size will be SizeMax
type: float
default value: 10
DistMin
Value up to which the mesh size will be SizeMin
type: float
default value: 1
InField
Tag of the field computing the input value, usually a distance
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
Mesh size when value > DistMax
type: float
default value: 1
SizeMin
Mesh size when value < DistMin
type: float
default value: 0.1
StopAtDistMax
True to not impose mesh size outside DistMax (i.e., F = a very big value if Field[InField] > DistMax)
type: boolean
default value: 0
Next: Miscellaneous mesh commands, Previous: Specifying mesh element sizes, Up: Mesh commands [Contents][Index]
Extrude { expression-list } { extrude-list layers }
Extrude 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, 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 }
Extrude 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 }
Extrude 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; > }
Extrude 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 >;
Select 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 > ;
Select 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 } > ;
Select 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 } ;
Apply 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;
Generate expression-D mesh. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
TransformMesh { expression-list };
Transform all the node coordinates in the current mesh using the 4x4 affine transformation matrix given by row (only 12 entries can be provided for convenience).
TransformMesh { expression-list } { transform-list };
Transform the node coordinates in the current mesh of all the elementary entities in transform-list using the 4x4 affine transformation matrix given by row (only 12 entries can be provided for convenience).
RefineMesh;
Refine 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;
Optimize 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 < , … > } };
Perform adaptive mesh generation. Documentation not yet available.
RelocateMesh Point | Curve | Surface { expression-list-or-all };
Relocate 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;
Change the order of the elements in the current mesh.
PartitionMesh expression;
Partition the mesh into expression, using current partitioning options.
Point | Curve { expression-list } In Surface { expression };
Add a meshing constraint to 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 };
Add a meshing constraint to 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 algorithms. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
Periodic Curve { expression-list } = { expression-list } ;
Add a meshing constraint to 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 } ;
Add a meshing constraint to 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 } ;
Add a meshing constraint to 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 } ;
Add a meshing constraint to 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;
Remove all duplicate mesh nodes in the current mesh.
CreateTopology < { expression , expression } > ;
Create 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 }; … } > ;
Create a geometry for discrete entities (represented solely by a mesh, without an underlying CAD description) in the current model, 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 current 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;
Renumber the node tags in the current mesh in a contiunous sequence.
RenumberMeshElements;
Renumber the elements tags in the current mesh in a contiunous sequence.
< Recursive > Color color-expression { <Physical> Point | Curve | Surface | Volume { expression-list-or-all }; … }
Set 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.
Recombine Surface { expression-list-or-all } < = expression >;
Recombine 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;
Specify the meshing algorithm for the surfaces expression-list.
MeshSizeFromBoundary Surface { expression-list } = expression;
Force the mesh size to be extended from the boundary (or not, depening on the value of expression) for the surfaces expression-list.
Compound Curve | Surface { expression-list-or-all } ;
Treat 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 } ;
Add a constraint to reverse the orientation of the mesh of the given curve(s) or surface(s) during meshing. This operation triggers a synchronization of the CAD model with the internal Gmsh model.
ReorientMesh Volume { expression-list } ;
Add a constraint to reorient the meshes (during mesh generation) of the bounding surfaces of the given volumes so that the normals point outward to the volumes; and if a mesh already exists, reorient it. 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;
Save the current 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.
Smoother Surface { expression-list } = expression;
Set the 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: Top [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: Top [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, and t9).
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
tutorials
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.
• Post-processing commands | ||
• Post-processing plugins | ||
• Post-processing options |
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];
Create 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];
Create 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;
Combine 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;
Combine 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;
Combine 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;
Combine 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;
Combine 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;
Combine 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];
Delete (remove) the expression-th post-processing view. Note that post-processing view indices start at 0.
Delete Empty Views;
Delete (remove) all the empty post-processing views.
Background Mesh View[expression];
Apply the expression-th post-processing view as the current background mesh. Note that post-processing view indices start at 0.
Plugin (string) . Run;
Execute the plugin string. The list of default plugins is given in Post-processing plugins.
Plugin (string) . string = expression | char-expression;
Set an option for a given plugin. See Post-processing plugins, for a list of default plugins and t9, for some examples.
Save View[expression] char-expression;
Save 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;
Send the expression-th post-processing view to the ONELAB server, with parameter name char-expression.
View "string" { string < ( expression-list ) > { expression-list }; … };
Create 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), 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 positive 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. If ‘AuxiliaryPhysicalGroup’ is given (> 0), its elements are considered in addition to those in ‘PhysicalGroup’ for the logic that groups the elements into the positive and negative side of the crack. However, the nodes in ‘AuxiliaryPhysicalGroup’ are not duplicated (unless they are also in ‘PhysicalGroup’). This can be useful to treat corner cases in non-trivial geometries. For 1D cracks, ‘NormalX’, ‘NormalY’ and ‘NormalZ’ provide the reference normal of the surface in which the crack is supposed to be embedded. If ‘NewPhysicalGroup’ is positive, use it as the tag of the newly created curve or surface; otherwise use ‘PhysicalGroup’. Numeric options:
Dimension
Default value: 1
PhysicalGroup
Default value: 1
OpenBoundaryPhysicalGroup
Default value: 0
AuxiliaryPhysicalGroup
Default value: 0
NormalX
Default value: 0
NormalY
Default value: 0
NormalZ
Default value: 1
NewPhysicalGroup
Default value: 0
DebugView
Default value: 0
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: 3
TargetError
Default value: 0.0001
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: 3
TargetError
Default value: 0.0001
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. If the bounding box defined by ‘XMin’ < x < ‘XMax, ‘YMin’ < y < ‘YMax and ‘ZMin’ < z < ‘ZMax’ is not empty, mark all elements outside the bounding box as invisible prior to deleting or inverting the elements. Numeric options:
DeleteElements
Default value: 1
ReverseElements
Default value: 0
XMin
Default value: 0
YMin
Default value: 0
ZMin
Default value: 0
XMax
Default value: 0
YMax
Default value: 0
ZMax
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: 3
TargetError
Default value: 0.0001
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 elements 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 distribution 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.) 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
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 different 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.
If ‘View’ < 0, the plugin is run on the current view.
Plugin(Triangulate) creates one new list-based view.
Numeric options:
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, and t9, for some examples.
Next: Tutorial, Previous: Post-processing module, Up: Top [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.)
• MSH file format | ||
• Node ordering | ||
• Legacy formats |
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.
• MSH file format version 2 (Legacy) | ||
• MSH file format version 1 (Legacy) | ||
• POS ASCII file format (Legacy) | ||
• POS binary file format (Legacy) |
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: Top [Contents][Index]
The following tutorials introduce new features gradually, starting with
t1. The corresponding files are available in the
tutorials
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 tutorials.
• t1 | Geometry basics, elementary entities, physical groups | |
• t2 | Transformations, extruded geometries, volumes | |
• t3 | Extruded meshes, ONELAB parameters, options | |
• t4 | Built-in functions, holes in surfaces, annotations, entity colors | |
• t5 | Mesh sizes, macros, loops, holes in volumes | |
• t6 | Transfinite meshes | |
• t7 | Background meshes | |
• t8 | Post-processing and animations | |
• t9 | Plugins | |
• t10 | Mesh size fields | |
• t11 | Unstructured quadrangular meshes | |
• t12 | Cross-patch meshing with compounds | |
• t13 | Remeshing an STL file without an underlying CAD model | |
• t14 | Homology and cohomology computation | |
• t15 | Embedded points, lines and surfaces | |
• t16 | Constructive Solid Geometry, OpenCASCADE geometry kernel | |
• t17 | Anisotropic background mesh | |
• t18 | Periodic meshes | |
• t19 | Thrusections, fillets, pipes, mesh size from curvature | |
• t20 | STEP import and manipulation, geometry partitioning | |
• t21 | Mesh partitioning | |
• x1 | Geometry and mesh data | |
• x2 | Mesh import, discrete entities, hybrid models, terrain meshing | |
• x3 | Post-processing data import: list-based | |
• x4 | Post-processing data import: model-based | |
• x5 | Additional geometrical data: parametrizations, normals, curvatures | |
• x6 | Additional mesh data: integration points, Jacobians and basis functions | |
• x7 | Additional mesh data: internal edges and faces |
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 `examples/boolean' for more.
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.
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'.
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 }; }
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 `newc', `newcl, `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 = newcl; Curve Loop(l1) = {c5,c10,c4}; l2 = newcl; Curve Loop(l2) = {c9,-c5,c1}; l3 = newcl; Curve Loop(l3) = {c12,-c8,-c1}; l4 = newcl; Curve Loop(l4) = {c8,-c4,c11}; l5 = newcl; Curve Loop(l5) = {-c10,c6,c3}; l6 = newcl; Curve Loop(l6) = {-c11,-c3,c7}; l7 = newcl; Curve Loop(l7) = {-c2,-c7,-c12}; l8 = newcl; 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;
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 = newc; Line(l1) = {1, p1}; l2 = newc; Line(l2) = {p1, p2}; l3 = newc; 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;
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".
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-%g.gif", num2); // Print Sprintf("t8-%g.ppm", num2); // Print Sprintf("t8-%g.jpg", num2); EndIf EndFor If(num == 3) // Here we could make a system call to generate a movie. For example, with // ffmpeg: // System "ffmpeg -i t8-%d.jpg t8.mpg" EndIf EndFor
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;
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].Sampling = 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; Field[6].Thickness = 0.3; // 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. // 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 are interpolated inside surfaces and/or volumes depending // on the value of `Mesh.MeshSizeExtendFromBoundary' (which is set 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. // Finally, while the default "Frontal-Delaunay" 2D meshing algorithm // (Mesh.Algorithm = 6) usually leads to the highest quality meshes, the // "Delaunay" algorithm (Mesh.Algorithm = 5) will handle complex mesh size // fields better - in particular size fields with large element size gradients: Mesh.Algorithm = 5;
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;
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};
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;
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.
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 = newc; 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 = newcl; 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};
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 // `examples/boolean' directory.
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) = {-2, -2, 0, 4, 4}; // 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;
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
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;
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'.
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
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()
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()
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()
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 constructed 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()
x5
: Additional geometrical data: parametrizations, normals, curvaturesSee x5.py. Also available in C++ (x5.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 5 # # Additional geometrical data: parametrizations, normals, curvatures # # ----------------------------------------------------------------------------- import gmsh import sys import math gmsh.initialize(sys.argv) # The API provides access to geometrical data in a CAD kernel agnostic manner. # Let's create a simple CAD model by fusing a sphere and a cube, then mesh the # surfaces: gmsh.model.add("x5") s = gmsh.model.occ.addSphere(0, 0, 0, 1) b = gmsh.model.occ.addBox(0.5, 0, 0, 1.3, 2, 3) gmsh.model.occ.fuse([(3, s)], [(3, b)]) gmsh.model.occ.synchronize() gmsh.model.mesh.generate(2) # We can for example retrieve the exact normals and the curvature at all the # mesh nodes (i.e. not normals and curvatures computed from the mesh, but # directly evaluated on the geometry), by querying the CAD kernels at the # corresponding parametric coordinates. normals = [] curvatures = [] # For each surface in the model: for e in gmsh.model.getEntities(2): # Retrieve the surface tag s = e[1] # Get the mesh nodes on the surface, including those on the boundary # (contrary to internal nodes, which store their parametric coordinates, # boundary nodes will be reparametrized on the surface in order to compute # their parametric coordinates, the result being different when # reparametrized on another adjacent surface) tags, coord, param = gmsh.model.mesh.getNodes(2, s, True) # Get the surface normals on all the points on the surface corresponding to # the parametric coordinates of the nodes norm = gmsh.model.getNormal(s, param) # In the same way, get the curvature curv = gmsh.model.getCurvature(2, s, param) # Store the normals and the curvatures so that we can display them as # list-based post-processing views for i in range(0, len(coord), 3): normals.append(coord[i]) normals.append(coord[i + 1]) normals.append(coord[i + 2]) normals.append(norm[i]) normals.append(norm[i + 1]) normals.append(norm[i + 2]) curvatures.append(coord[i]) curvatures.append(coord[i + 1]) curvatures.append(coord[i + 2]) curvatures.append(curv[i // 3]) # Create a list-based vector view on points to display the normals, and a scalar # view on points to display the curvatures vn = gmsh.view.add("normals") gmsh.view.addListData(vn, "VP", len(normals) // 6, normals) vc = gmsh.view.add("curvatures") gmsh.view.addListData(vc, "SP", len(curvatures) // 4, curvatures) # We can also retrieve the parametrization bounds of model entities, e.g. of # curve 5, and evaluate the parametrization for several parameter values: bounds = gmsh.model.getParametrizationBounds(1, 5) N = 20 t = [bounds[0][0] + i * (bounds[1][0] - bounds[0][0]) / N for i in range(N)] xyz1 = gmsh.model.getValue(1, 5, t) # We can also reparametrize curve 5 on surface 1, and evaluate the points in the # parametric plane of the surface: uv = gmsh.model.reparametrizeOnSurface(1, 5, t, 1) xyz2 = gmsh.model.getValue(2, 1, uv) # Hopefully we get the same x, y, z coordinates! if max([abs(a - b) for (a, b) in zip(xyz1, xyz2)]) < 1e-12: gmsh.logger.write('Evaluation on curve and surface match!') else: gmsh.logger.write('Evaluation on curve and surface do not match!', 'error') # Launch the GUI to see the results: if '-nopopup' not in sys.argv: gmsh.fltk.run() gmsh.finalize()
x6
: Additional mesh data: integration points, Jacobians and basis functionsSee x6.py. Also available in C++ (x6.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 6 # # Additional mesh data: integration points, Jacobians and basis functions # # ----------------------------------------------------------------------------- import gmsh import sys gmsh.initialize(sys.argv) gmsh.model.add("x6") # The API provides access to all the elementary building blocks required to # implement finite-element-type numerical methods. Let's create a simple 2D # model and mesh it: gmsh.model.occ.addRectangle(0, 0, 0, 1, 0.1) gmsh.model.occ.synchronize() gmsh.model.mesh.setTransfiniteAutomatic() gmsh.model.mesh.generate(2) # Set the element order and the desired interpolation order: elementOrder = 1 interpolationOrder = 2 gmsh.model.mesh.setOrder(elementOrder) def pp(label, v, mult): print(" * " + str(len(v) / mult) + " " + label + ": " + str(v)) # Iterate over all the element types present in the mesh: elementTypes = gmsh.model.mesh.getElementTypes() for t in elementTypes: # Retrieve properties for the given element type elementName, dim, order, numNodes, numPrimNodes, localNodeCoord =\ gmsh.model.mesh.getElementProperties(t) print("\n** " + elementName + " **\n") # Retrieve integration points for that element type, enabling exact # integration of polynomials of order "interpolationOrder". The "Gauss" # integration family returns the "economical" Gauss points if available, and # defaults to the "CompositeGauss" (tensor product) rule if not. localCoords, weights =\ gmsh.model.mesh.getIntegrationPoints(t, "Gauss" + str(interpolationOrder)) pp("integration points to integrate order " + str(interpolationOrder) + " polynomials", localCoords, 3) # Return the basis functions evaluated at the integration points. Selecting # "Lagrange" and "GradLagrange" returns the isoparamtric basis functions and # their gradient (in the reference space of the given element type). A # specific interpolation order can be requested using "LagrangeN" and # "GradLagrangeN" with N = 1, 2, ... Other supported function spaces include # "H1LegendreN", "GradH1LegendreN", "HcurlLegendreN", "CurlHcurlLegendreN". numComponents, basisFunctions, numOrientations =\ gmsh.model.mesh.getBasisFunctions(t, localCoords, "Lagrange") pp("basis functions at integration points", basisFunctions, 1) numComponents, basisFunctions, numOrientations =\ gmsh.model.mesh.getBasisFunctions(t, localCoords, "GradLagrange") pp("basis function gradients at integration points", basisFunctions, 3) # Compute the Jacobians (and their determinants) at the integration points # for all the elements of the given type in the mesh. Beware that the # Jacobians are returned "by column": see the API documentation for details. jacobians, determinants, coords =\ gmsh.model.mesh.getJacobians(t, localCoords) pp("Jacobian determinants at integration points", determinants, 1) gmsh.finalize()
x7
: Additional mesh data: internal edges and facesSee x7.py. Also available in C++ (x7.cpp).
# ----------------------------------------------------------------------------- # # Gmsh Python extended tutorial 7 # # Additional mesh data: internal edges and faces # # ----------------------------------------------------------------------------- import sys import gmsh gmsh.initialize(sys.argv) gmsh.model.add("x7") # Meshes are fully described in Gmsh by nodes and elements, both associated to # model entities. The API can be used to generate and handle other mesh # entities, i.e. mesh edges and faces, which are not stored by default. # Let's create a simple model and mesh it: gmsh.model.occ.addBox(0, 0, 0, 1, 1, 1) gmsh.model.occ.synchronize() gmsh.option.setNumber("Mesh.MeshSizeMin", 2.) gmsh.model.mesh.generate(3) # Like elements, mesh edges and faces are described by (an ordered list of) # their nodes. Let us retrieve the edges and the (triangular) faces of all the # first order tetrahedra in the mesh: elementType = gmsh.model.mesh.getElementType("tetrahedron", 1) edgeNodes = gmsh.model.mesh.getElementEdgeNodes(elementType) faceNodes = gmsh.model.mesh.getElementFaceNodes(elementType, 3) # Edges and faces are returned for each element as a list of nodes corresponding # to the canonical orientation of the edges and faces for a given element type. # Gmsh can also identify unique edges and faces (a single edge or face whatever # the ordering of their nodes) and assign them a unique tag. This identification # can be done internally by Gmsh (e.g. when generating keys for basis # functions), or requested explicitly as follows: gmsh.model.mesh.createEdges() gmsh.model.mesh.createFaces() # Edge and face tags can then be retrieved by providing their nodes: edgeTags, edgeOrientations = gmsh.model.mesh.getEdges(edgeNodes) faceTags, faceOrientations = gmsh.model.mesh.getFaces(3, faceNodes) # Since element edge and face nodes are returned in the same order as the # elements, one can easily keep track of which element(s) each edge or face is # connected to: elementTags, elementNodeTags = gmsh.model.mesh.getElementsByType(elementType) edges2Elements = {} faces2Elements = {} for i in range(len(edgeTags)): # 6 edges per tetrahedron if not edgeTags[i] in edges2Elements: edges2Elements[edgeTags[i]] = [elementTags[i // 6]] else: edges2Elements[edgeTags[i]].append(elementTags[i // 6]) for i in range(len(faceTags)): # 4 faces per tetrahedron if not faceTags[i] in faces2Elements: faces2Elements[faceTags[i]] = [elementTags[i // 4]] else: faces2Elements[faceTags[i]].append(elementTags[i // 4]) # New unique lower dimensional elements can also be easily created given the # edge or face nodes. This is especially useful for numerical methods that # require integrating or interpolating on internal edges or faces (like # e.g. Discontinuous Galerkin techniques), since creating elements for the # internal entities will make this additional mesh data readily available (see # `x6.py'). For example, we can create a new discrete surface... s = gmsh.model.addDiscreteEntity(2) # ... and fill it with unique triangles corresponding to the faces of the # tetrahedra: maxElementTag = gmsh.model.mesh.getMaxElementTag() uniqueFaceTags = set() tagsForTriangles = [] faceNodesForTriangles = [] for i in range(len(faceTags)): if faceTags[i] not in uniqueFaceTags: uniqueFaceTags.add(faceTags[i]) tagsForTriangles.append(faceTags[i] + maxElementTag) faceNodesForTriangles.append(faceNodes[3 * i]) faceNodesForTriangles.append(faceNodes[3 * i + 1]) faceNodesForTriangles.append(faceNodes[3 * i + 2]) elementType2D = gmsh.model.mesh.getElementType("triangle", 1) gmsh.model.mesh.addElementsByType(s, elementType2D, tagsForTriangles, faceNodesForTriangles) # Since the tags for the triangles have been created based on the face tags, # the information about neighboring elements can also be readily created, # useful e.g. in Finite Volume or Discontinuous Galerkin techniques: for t in tagsForTriangles: print("triangle " + str(int(t)) + " is connected to tetrahedra " + str(faces2Elements[t - maxElementTag])) # If all you need is the list of all edges or faces in terms of their nodes, you # can also directly call: edgeTags, edgeNodes = gmsh.model.mesh.getAllEdges() faceTags, faceNodes = gmsh.model.mesh.getAllFaces(3) # Launch the GUI to see the results: if '-nopopup' not in sys.argv: gmsh.fltk.run()
Next: Compiling the source code, Previous: Tutorial, Up: Top [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).
• General options list | ||
• Geometry options list | ||
• Mesh options list | ||
• Solver options list | ||
• Post-processing options list |
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: 4.10.2-git-f32ab4d30; License: GNU General Public License; Build OS: MacOSX-sdk; Build date: 20220509; Build host: MacBook-Pro-Christophe.local; Build options: 64Bit ALGLIB[contrib] ANN[contrib] Bamg Blossom Cairo Cgns DIntegration Dlopen DomHex Eigen[contrib] Fltk GMP Gmm[contrib] Hxt Jpeg Kbipack MathEx[contrib] Med Mesh Metis[contrib] Mmg Mpeg Netgen ONELAB ONELABMetamodel OpenCASCADE OpenCASCADE-CAF OpenGL OpenMP OptHom Parasolid ParasolidSTEP Parser Plugins Png Post QuadMeshingTools QuadTri Solver TetGen/BR TouchBar Voro++[contrib] WinslowUntangler Zlib; FLTK version: 1.4.0; OCC version: 7.7.0; MED version: 4.1.1; 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[contrib] ANN[contrib] Bamg Blossom Cairo Cgns DIntegration Dlopen DomHex Eigen[contrib] Fltk GMP Gmm[contrib] Hxt Jpeg Kbipack MathEx[contrib] Med Mesh Metis[contrib] Mmg Mpeg Netgen ONELAB ONELABMetamodel OpenCASCADE OpenCASCADE-CAF OpenGL OpenMP OptHom Parasolid ParasolidSTEP Parser Plugins Png Post QuadMeshingTools QuadTri Solver TetGen/BR TouchBar Voro++[contrib] WinslowUntangler 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: "4.10.2-git-f32ab4d30"
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.DetachedProcess
On Windows, should processes created by Gmsh be detached?
Default value: 1
Saved in: General.OptionsFileName
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
Maximum number of threads used by Gmsh when compiled with OpenMP support (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.X3dVolumes
Save separate volumes in CAD X3D output (0: no, 1: yes)
Default value: 0
Saved in: General.OptionsFileName
Print.X3dColorize
Apply colors to faces (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 the default OpenCASCADE behavior); the option should be set before importing the STEP or IGES file
Default value: ""
Saved in: General.OptionsFileName
Geometry.PipeDefaultTrihedron
Default trihedron type when creating pipes
Default value: "DiscreteTrihedron"
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 and boundary curves and surfaces?
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.OCCAutoEmbed
Automatically embed points, curves and faces in higher dimensional entities if they are marked as ’internal’ by OpenCASCADE
Default value: 1
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.OCCSafeUnbind
Revert to safe (i.e. with recursive checks on boundaries) unbinding of entities in boolean operations and geometrical transformations
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 explicitly 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.OrientedPhysicals
Use sign of elementary entity in physical definition as orientation indicator
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.SnapPoints
Snap points on curves if their evaluation using the parametrization is larger than the geometrical tolerance (currently only with the OpenCASCADE kernel)
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, 11: Quasi-structured Quad)
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 when generating or renumbering a mesh
Default value: 1
Saved in: General.OptionsFileName
Mesh.FirstNodeTag
First tag (>= 1) of mesh nodes when generating or renumbering a mesh
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.HighOrderFixBoundaryNodes
Fix boundary nodes during high-order optimization?
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 alignment 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 General.NumThreads)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MaxNumThreads2D
Maximum number of threads for 2D meshing (0: use General.NumThreads)
Default value: 0
Saved in: General.OptionsFileName
Mesh.MaxNumThreads3D
Maximum number of threads for 3D meshing (0: use General.NumThreads)
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 (0: never; 1: for surfaces and volumes; 2: for surfaces and volumes, but use smallest surface element edge length instead of longest length in 3D Delaunay; -2: only for surfaces; -3: only for volumes)
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.MinimumLineNodes
Minimum number of nodes used to mesh (straight) lines
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.OldInitialDelaunay2D
Use old initial 2D Delaunay code
Default value: 0
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.QuadqsSizemapMethod
Size map method in QuadQuasiStructured. 0: default, 1: cross-field,2: cross-field + CAD small features adaptation,3: from background mesh (e.g. sizes in current triangulation),4: cross-field + CAD small features adaptation (clamped by background mesh)
Default value: 3
Saved in: General.OptionsFileName
Mesh.QuadqsTopologyOptimizationMethods
Topology optimization methods in QuadQuasiStructured. 0: default (all),100: pattern-based CAD faces,010: disk quadrangulation remeshing,001: cavity remeshing,xxx: combination of multiple methods (e.g. 111 for all)
Default value: 0
Saved in: General.OptionsFileName
Mesh.QuadqsRemeshingBoldness
Controls how much cavity remeshing is allowed to distort the quad mesh. From 0 (no quality decrease during remeshing) to 1 (quality can tend to 0 during remeshing).
Default value: 0.66
Saved in: General.OptionsFileName
Mesh.QuadqsScalingOnTriangulation
Ratio on the edge length between the triangulation and the quadrangulation. Use a small ratio (e.g. 0.5) to get a background triangulation finer than the quad mesh. Useful to get a more accurate cross-field.
Default value: 0.75
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.RecombineNodeRepositioning
Allow repositioning of nodes during recombination of surface meshes
Default value: 1
Saved in: General.OptionsFileName
Mesh.RecombineMinimumQuality
Minimum quality for quadrangle generated by recombination
Default value: 0
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) if value is positive; if negative, save groups of elements for physical groups of dimension dim if the (dim+1)^th least significant digit of -Mesh.SaveGroupsOfElements is 1 (for example: -100 will only savesurfaces, while -1010 will save volumes and curves), and for INP skip saving elements of dimension dim altogether if the (dim+1)^th least significant digit of -Mesh.SaveGroupsOfElements is 0
Default value: 1
Saved in: General.OptionsFileName
Mesh.SaveGroupsOfNodes
Save groups of nodes for each physical group (for UNV, INP and Tochnog mesh formats) if value is positive; if negative, save groups of nodes for physical groups of dimension dim if the (dim+1)^th least significant digit of -Mesh.SaveGroupsOfNodes is 1 (for example: -100 will only save surfaces, while -1010 will save volumes and curves); for INP, save groups of nodes for all entities of dimension dim if the (dim+1)^th least significant digit of -Mesh.SaveGroupsOfNodes is 2
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 representations of entities (currently only used with the OpenCASCADE kernel)
Default value: 0.3
Saved in: General.OptionsFileName
Mesh.StlLinearDeflection
Maximum relative linear deflection when creating STL representation of entities (currently only used with the OpenCASCADE kernel)
Default value: 0.001
Saved in: General.OptionsFileName
Mesh.StlLinearDeflectionRelative
Compute the linear deflection for STL representations relative to the length of curves (currently only used with the OpenCASCADE kernel)
Default value: 1
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-12
Saved in: General.OptionsFileName
Mesh.ToleranceReferenceElement
Tolerance for classifying a point inside a reference element (of size 1)
Default value: 1e-06
Saved in: General.OptionsFileName
Mesh.Triangles
Display mesh triangles?
Default value: 1
Saved in: General.OptionsFileName
Mesh.Trihedra
Display mesh trihedra?
Default value: 1
Saved in: General.OptionsFileName
Mesh.TransfiniteTri
Use alternative transfinite arrangement when meshing 3-sided surfaces
Default value: 0
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.Binary
Write post-processing files in binary format (if possible)
Default value: 0
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: 0.0001
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_GEOMETRYCENTRAL
Enable geometry-central library (experimental) (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 (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: ON)
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_QUADMESHINGTOOLS
Enable QuadMeshingTools 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_WINSLOWUNTANGLER
Enable WinslowUntangler extensions (requires ALGLIB) (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: Top [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 tutorials/c++, tutorials/c, tutorials/python and tutorials/julia directories from the Tutorial for examples. For other API examples, see the examples/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/parser
(which handles the Gmsh parser),
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.
Next: Namespace gmsh/option, Up: Gmsh API [Contents][Index]
gmsh
: top-level functionsgmsh/initialize
Initialize the 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). If run
is set,
run in the same way as the Gmsh app, either interactively or in batch mode
depending on the command line arguments. If run
is not set, initializing
the API sets the options "General.AbortOnError" to 2 and "General.Terminal" to
1. If compiled with OpenMP support, it also sets the number of threads to
"General.NumThreads".
gmsh/isInitialized
Return 1 if the Gmsh API is initialized, and 0 if not.
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), Python (x1.py, explore.py, flatten2.py, flatten.py, heal.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, Previous: Namespace gmsh, 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.Color.Option" or
"Category[num].Color.Option". Available categories and options are listed in the
Gmsh reference manual. For conciseness "Color." can be ommitted in name
.
gmsh/option/getColor
Get the r
, g
, b
, a
value of a color option.
name
is of the form "Category.Color.Option" or
"Category[num].Color.Option". Available categories and options are listed in the
Gmsh reference manual. For conciseness "Color." can be ommitted in name
.
Next: Namespace gmsh/model/mesh, Previous: Namespace gmsh/option, 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. Set the name of the
physical group if name
is not empty.
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
.
dim
, tag
, name
-
-
Python (poisson.py, step_assembly.py)
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/setTag
Set the tag of the entity of dimension dim
and tag tag
to the new
value newTag
.
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
Return 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.
gmsh/model/removeEntities
Remove the entities dimTags
of the current model, provided that they are
not on the boundary of (or embedded in) higher-dimensional entities. 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), Python (t21.py, x1.py, explore.py, partition.py, tube_hole_boundary_layer.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), Python (t21.py, x1.py, explore.py, partition.py)
gmsh/model/getNumberOfPartitions
Return the number of partitions in the model.
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), 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, x5.cpp), Python (t2.py, x5.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, ...]).
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, ...].
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
.
gmsh/model/isInside
Check if the coordinates (or the parametric coordinates if parametric
is
set) provided in coord
correspond to points inside the entity of
dimension dim
and tag tag
, and return the number of points inside.
This feature is only available for a subset of entities, depending on the
underlying 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 underlying geometrical representation.
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, Previous: Namespace gmsh/model, 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.
Optionally, elementTags
and partitions
can be provided to specify
the partition of each element explicitly.
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,
"QuadQuasiStructured" for quad mesh optimization, "UntangleMeshGeometry" for
untangling). If force
is set apply the optimization also to discrete
entities. If dimTags
is given, only apply the optimizer to the given
entities.
method = ""
, force = False
, niter = 1
, dimTags = []
-
-
Python (naca_boundary_layer_2d.py, naca_boundary_layer_3d.py, opt.py, tube_boundary_layer.py)
gmsh/model/mesh/recombine
Recombine the mesh of the current model.
-
-
-
Python (stl_to_mesh.py)
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
-
-
C++ (x6.cpp), Python (x6.py, hybrid_order.py, naca_boundary_layer_2d.py, naca_boundary_layer_3d.py, tube_boundary_layer.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/reverse
Reverse the orientation of the elements in the entities dimTags
. If
dimTags
is empty, reverse the orientation of the elements in the whole
mesh.
dimTags = []
-
-
Python (mirror_mesh.py)
gmsh/model/mesh/affineTransform
Apply the affine transformation affineTransform
(16 entries of a 4x4
matrix, by row; only the 12 first can be provided for convenience) to the
coordinates of the nodes classified on the entities dimTags
. If
dimTags
is empty, transform all the nodes in the mesh.
affineTransform
, dimTags = []
-
-
Python (flatten2.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).
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
.
elementType
, tag = -1
, returnParametricCoord = True
nodeTags
, coord
, parametricCoord
-
Python (stl_to_brep.py)
gmsh/model/mesh/getNode
Get the coordinates and the parametric coordinates (if any) of the node with tag
tag
, as well as the dimension dim
and tag tag
of the entity
on which the node is classified. 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/getMaxNodeTag
Get the maximum tag maxTag
of a node in the mesh.
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), 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), Python (x1.py, copy_mesh.py, explore.py, flatten.py, mesh_quality.py, ...)
gmsh/model/mesh/getElement
Get the type and node tags of the element with tag tag
, as well as the
dimension dim
and tag tag
of the entity on which the element is
classified. 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), Python (x1.py, x6.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++ (x7.cpp), Python (x7.py, adapt_mesh.py, neighbors.py, poisson.py, stl_to_brep.py)
gmsh/model/mesh/getMaxElementTag
Get the maximum tag maxTag
of an element in the mesh.
gmsh/model/mesh/preallocateElementsByType
Preallocate data before calling getElementsByType
with numTasks
>
1. For C and C++ only.
gmsh/model/mesh/getElementQualities
Get the quality elementQualities
of the elements with tags
elementTags
. qualityType
is the requested quality measure: "minSJ"
for the minimal scaled jacobien, "minSICN" for the minimal signed inverted
condition number, "minSIGE" for the signed inverted gradient error, "gamma" for
the ratio of the inscribed to circumcribed sphere radius, "volume" for the
volume. If numTasks
> 1, only compute and return the part of the data
indexed by task
.
elementTags
, qualityName = "minSICN"
, task = 0
, numTasks = 1
elementsQuality
-
Python (mesh_quality.py)
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
-
-
Python (copy_mesh.py, discrete.py, flatten.py, mesh_from_discrete_curve.py, mirror_mesh.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.
gmsh/model/mesh/getIntegrationPoints
Get the numerical quadrature information for the given element type
elementType
and integration rule integrationType
, where
integrationType
concatenates the integration rule family name with the
desired order (e.g. "Gauss4" for a quadrature suited for integrating 4th order
polynomials). The "CompositeGauss" family uses tensor-product rules based the 1D
Gauss-Legendre rule; the "Gauss" family uses an economic scheme when available
(i.e. with a minimal number of points), and falls back to "CompositeGauss"
otherwise. Note that integration points for the "Gauss" family can fall outside
of the reference element for high-order rules. 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
-
Python (x6.py, 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
-
Python (x6.py, 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
. Currently supported function spaces
include "Lagrange" and "GradLagrange" for isoparametric Lagrange basis functions
and their gradient in the u, v, w coordinates of the reference element;
"LagrangeN" and "GradLagrangeN", with N = 1, 2, ..., for N-th order Lagrange
basis functions; "H1LegendreN" and "GradH1LegendreN", with N = 1, 2, ..., for
N-th order hierarchical H1 Legendre functions; "HcurlLegendreN" and
"CurlHcurlLegendreN", with N = 1, 2, ..., for N-th order curl-conforming basis
functions. numComponents
returns the number C of components of a basis
function (e.g. 1 for scalar functions and 3 for vector functions).
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
-
Python (x6.py, adapt_mesh.py, poisson.py)
gmsh/model/mesh/getBasisFunctionsOrientation
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/preallocateBasisFunctionsOrientation
Preallocate data before calling getBasisFunctionsOrientation
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
. Mesh edges are created e.g. by
createEdges()
, getKeys()
or addEdges()
. The reference
positive orientation is n1 < n2, where n1 and n2 are the tags of the two edge
nodes, which corresponds to the local orientation of edge-based basis functions
as well.
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
. Mesh faces are created e.g.
by createFaces()
, getKeys()
or addFaces()
.
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/getAllEdges
Get the global unique identifiers edgeTags
and the nodes edgeNodes
of the edges in the mesh. Mesh edges are created e.g. by createEdges()
,
getKeys()
or addEdges().
gmsh/model/mesh/getAllFaces
Get the global unique identifiers faceTags
and the nodes faceNodes
of the faces of type faceType
in the mesh. Mesh faces are created e.g. by
createFaces()
, getKeys()
or addFaces().
gmsh/model/mesh/addEdges
Add mesh edges defined by their global unique identifiers edgeTags
and
their nodes edgeNodes
.
gmsh/model/mesh/addFaces
Add mesh faces of type faceType
defined by their global unique
identifiers faceTags
and their nodes faceNodes
.
gmsh/model/mesh/getKeys
Generate the pair of keys for the elements of type elementType
in the
entity of tag tag
, for the functionSpaceType
function space. Each
pair (typeKey
, entityKey
) 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 pair of keys for a single element elementTag
.
gmsh/model/mesh/getNumberOfKeys
Get the number of keys by elements of type elementType
for function space
named functionSpaceType
.
gmsh/model/mesh/getKeysInformation
Get information about the pair of keys
. infoKeys
returns
information about the functions associated with the pairs (typeKeys
,
entityKey
). 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.
gmsh/model/mesh/getSizes
Get the mesh size constraints (if any) associated with the model entities
dimTags
. A zero entry in the output sizes
vector indicates that no
size constraint is specified on the corresponding entity.
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 mesh size callback for the current model. The callback function should
take six arguments as input (dim
, tag
, x
, y
,
z
and lc
). The first two integer arguments correspond to the
dimension dim
and tag tag
of the entity being meshed. The next
four double precision arguments correspond to the coordinates x
, y
and z
around which to prescribe the mesh size and to the mesh size
lc
that would be prescribed if the callback had not been called. The
callback function should return a double precision number specifying the desired
mesh size; returning lc
is equivalent to a no-op.
gmsh/model/mesh/removeSizeCallback
Remove the mesh size callback from the current model.
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, tube_hole_boundary_layer.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), 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, tube_hole_boundary_layer.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; angle
specifies the
threshold angle for the simple recombination algorithm..
dim
, tag
, angle = 45.
-
-
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; and if a mesh
already exists, reorient it. 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.
-
-
-
Python (view_renumbering.py)
gmsh/model/mesh/renumberElements
Renumber the element tags in a continuous sequence.
-
-
-
Python (view_renumbering.py)
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/getPeriodic
Get master entities tagsMaster
for the entities of dimension dim
and tags tags
.
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/getPeriodicKeys
Get the master entity tagMaster
and the key pairs (typeKeyMaster
,
entityKeyMaster
) corresponding to the entity tag
and the key pairs
(typeKey
, entityKey
) for the elements of type elementType
and function space type functionSpaceType
. If returnCoord
is set,
the coord
and coordMaster
vectors contain the x, y, z coordinates
locating basis functions for sorting purposes.
elementType
, functionSpaceType
, tag
, returnCoord = True
tagMaster
, typeKeys
, typeKeysMaster
, entityKeys
, entityKeysMaster
, coord
, coordMaster
-
Python (periodic.py)
gmsh/model/mesh/importStl
Import the model STL representation (if available) as the current mesh.
-
-
-
Python (stl_to_mesh.py)
gmsh/model/mesh/getDuplicateNodes
Get the tags
of any duplicate nodes in the mesh of the entities
dimTags
. If dimTags
is empty, consider the whole mesh.
gmsh/model/mesh/removeDuplicateNodes
Remove duplicate nodes in the mesh of the entities dimTags
. If
dimTags
is empty, consider the whole mesh.
dimTags = []
-
-
Python (glue_and_remesh_stl.py, mirror_mesh.py, stl_to_mesh.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.
quality = 1.
, tag = -1
-