Gmsh 4.10.2

Table of Contents

Gmsh

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

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.

Copying conditions

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.

1 Overview

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.

1.1 Geometry: model entity creation

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.

1.2 Mesh: finite element mesh generation

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.

1.3 Solver: external solver interface

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.

1.4 Post-processing: scalar, vector and tensor field visualization

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).

1.5 What Gmsh is pretty good at …

Here is a tentative list of what Gmsh does best:

• quickly describe simple and/or “repetitive” geometries with the built-in scripting language, thanks to user-defined macros, loops, conditionals and includes (see User-defined macros, Loops and conditionals, and General commands). For more advanced geometries, using the Gmsh API (see Gmsh API) in the language of your choice (C++, C, Python or Julia) brings even greater flexibility, the only downside being that you need to either compile your code (for C++ and C) or to configure and install an interpreter (Python or Julia) in addition to Gmsh. A binary Software Development Kit (SDK) is distributed on the Gmsh web site to make the process easier;
• parametrize these geometries. Gmsh’s scripting language or the Gmsh API enable all commands and command arguments to depend on previous calculations (see Expressions, Geometry commands, and Gmsh API). Using the OpenCASCADE geometry kernel, Gmsh gives access to all usual constructive solid geometry operations;
• import geometries from other CAD software in standard exchange formats. Gmsh uses OpenCASCADE to import such files, including label and color information from STEP and IGES files;
• generate 1D, 2D and 3D simplicial (i.e., using line segments, triangles and tetrahedra) finite element meshes (see Mesh module), with fine control over the element size (see Specifying mesh element sizes);
• create simple extruded geometries and meshes (see Geometry commands, and Mesh commands), and allow to automatically couple such structured meshes with unstructured ones (using a layer of pyramids in 3D);
• generate high-order (curved) meshes that conform to the CAD model geometry. High-order mesh optimization tools allow to guarantee the validity of such curved meshes;
• interact with external solvers by defining ONELAB parameters, shared between Gmsh and the solvers and easily modifiable in the GUI (see Solver module);
• visualize and export computational results in a great variety of ways. Gmsh can display scalar, vector and tensor datasets, perform various operations on the resulting post-processing views (see Post-processing module), can export plots in many different formats (see General options list), and can generate complex animations (see General tools, and t8);
• run on low end machines and/or machines with no graphical interface. Gmsh can be compiled with or without the GUI (see Compiling the source code), and all versions can be used either interactively or directly from the command line (see Running Gmsh on your system);
• configure your preferred options. Gmsh has a large number of configuration options that can be set interactively using the GUI, scattered inside script files, changed through the API, set in per-user configuration files and specified on the command-line (see Running Gmsh on your system and Options);
• and do all the above on various platforms (Windows, Mac and Unix), for free (see Copying conditions)!

1.6 … and what Gmsh is not so good at

Here are some known weaknesses of Gmsh:

• Gmsh is not a multi-bloc mesh generator: all meshes produced by Gmsh are conforming in the sense of finite element meshes;
• Gmsh’s user interface is only exposing a limited number of the available features, and many aspects of the interface could be enhanced (especially manipulators).
• Your complaints about Gmsh here :-)

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!

1.7 Bug reports

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.

2 How to read this reference manual?

Gmsh can be used at three levels:

1. as a stand-alone application manipulated through its graphical user interface (GUI);
2. as a stand-alone script-driven application;
3. as a library.

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.

2.1 Syntactic rules used in the manual

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).

1. Keywords and literal symbols are printed like this.
2. Metasyntactic variables (i.e., text bits that are not part of the syntax, but stand for other text bits) are printed like this.
3. A colon (:) after a metasyntactic variable separates the variable from its definition.
4. Optional rules are enclosed in < > pairs.
5. Multiple choices are separated by |.
6. Three dots (…) indicate a possible (multiple) repetition of the preceding rule.

3 Running Gmsh on your system

3.1 Interactive mode

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.

3.2 Non-interactive mode

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;.

3.3 Command-line options

(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

3.4 Mouse actions

Move

Highlight the entity under the mouse pointer and display its properties / Resize a lasso zoom or a lasso (un)selection

Left button

Rotate / Select an entity / Accept a lasso zoom or a lasso selection

Ctrl+Left button

Start a lasso zoom or a lasso (un)selection

Middle button

Zoom / Unselect an entity / Accept a lasso zoom or a lasso unselection

Ctrl+Middle button

Orthogonalize display

Right button

Pan / Cancel a lasso zoom or a lasso (un)selection / Pop-up menu on post-processing view button

Ctrl+Right 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.

3.5 Keyboard shortcuts

(On Mac Ctrl is replaced by Cmd (the ‘Apple key’) in the shortcuts below.)

Left arrow

Go to previous time step

Right arrow

Go to next time step

Up arrow

Make previous view visible

Down arrow

Make next view visible

0

Reload geometry

Ctrl+0 or 9

Reload full project

1 or F1

Mesh lines

2 or F2

Mesh surfaces

3 or F3

Mesh volumes

Escape

Cancel lasso zoom/selection, toggle mouse selection ON/OFF

e

End/accept selection in geometry creation mode

g

Go to geometry module

m

Go to mesh module

p

Go to post-processing module

q

Abort selection in geometry creation mode

s

Go to solver module

x

Toggle x coordinate freeze in geometry creation mode

y

Toggle y coordinate freeze in geometry creation mode

z

Toggle z coordinate freeze in geometry creation mode

Shift+a

Bring all windows to front

Shift+g

Show geometry options

Shift+m

Show mesh options

Shift+o

Show general options

Shift+p

Show post-processing options

Shift+s

Show solver options

Shift+u

Show post-processing view plugins

Shift+w

Show post-processing view options

Shift+x

Move only along x coordinate in geometry creation mode

Shift+y

Move only along y coordinate in geometry creation mode

Shift+z

Move only along z coordinate in geometry creation mode

Shift+Escape

Enable full mouse selection

Ctrl+d

Attach/detach menu

Ctrl+e

Export project

Ctrl+f

Enter full screen

Ctrl+i

Show statistics window

Ctrl+j

Save model options

Ctrl+l

Show message console

Ctrl+m

Minimize window

Ctrl+n

Create new project file

Ctrl+o

Open project file

Ctrl+q

Quit

Ctrl+r

Rename project file

Ctrl+s

Save mesh in default format

Shift+Ctrl+c

Show clipping plane window

Shift+Ctrl+h

Show current options and workspace window

Shift+Ctrl+j

Save options as default

Shift+Ctrl+m

Show manipulator window

Shift+Ctrl+n

Show option window

Shift+Ctrl+o

Merge file(s)

Shift+Ctrl+r

Open next-to-last opened file

Shift+Ctrl+u

Show plugin window

Shift+Ctrl+v

Show visibility window

Alt+a

Loop through axes modes

Alt+b

Hide/show bounding boxes

Alt+c

Loop through predefined color schemes

Alt+e

Hide/Show element outlines for visible post-pro views

Alt+f

Change redraw mode (fast/full)

Alt+h

Hide/show all post-processing views

Alt+i

Hide/show all post-processing view scales

Alt+l

Hide/show geometry lines

Alt+m

Toggle visibility of all mesh entities

Alt+n

Hide/show all post-processing view annotations

Alt+o

Change projection mode (orthographic/perspective)

Alt+p

Hide/show geometry points

Alt+r

Loop through range modes for visible post-pro views

Alt+s

Hide/show geometry surfaces

Alt+t

Loop through interval modes for visible post-pro views

Alt+v

Hide/show geometry volumes

Alt+w

Enable/disable all lighting

Alt+x

Set X view

Alt+y

Set Y view

Alt+z

Set Z view

Alt+1

Set 1:1 view

Alt+Shift+a

Hide/show small axes

Alt+Shift+b

Hide/show mesh volume faces

Alt+Shift+c

Loop through predefined colormaps

Alt+Shift+d

Hide/show mesh surface faces

Alt+Shift+l

Hide/show mesh lines

Alt+Shift+p

Hide/show mesh nodes

Alt+Shift+s

Hide/show mesh surface edges

Alt+Shift+t

Same as Alt+t, but with numeric mode included

Alt+Shift+v

Hide/show mesh volume edges

Alt+Shift+x

Set -X view

Alt+Shift+y

Set -Y view

Alt+Shift+z

Set -Z view

Alt+Shift+1

Reset bounding box around visible entities

Alt+Ctrl++1

Sync scale between viewports

4 General tools

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.

4.1 Comments

Gmsh script files support both C and C++ style comments:

1. any text comprised between /* and */ pairs is ignored;
2. the rest of a line after a double slash // 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.

4.2 Expressions

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.

4.2.1 Floating point expressions

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.

4.2.2 Character expressions

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 <,…>

4.2.3 Color expressions

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.

4.3 Operators

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:

1. (), [], ., #
2. ^
3. !, ++, --, - (unary)
4. *, /, %
5. +, -
6. <, >, <=, >=
7. ==, !=
8. &&
9. ||
10. ?:
11. =, +=, -=, *=, /=

4.4 Built-in functions

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.

4.5 User-defined macros

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!

4.6 Loops and conditionals

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.

4.7 General commands

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:

1. If there is a mesh (i.e., at least one mesh node), the bounding box is taken as the box enclosing all the mesh nodes;
2. If there is no mesh but there is a geometry (i.e., at least one geometrical point), the bounding box is taken as the box enclosing all the geometrical points;
3. If there is no mesh and no geometry, but there are some post-processing views, the bounding box is taken as the box enclosing all the primitives in the views.

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.

4.8 General options

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.

5 Geometry module

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:

1. each point must possess a unique tag;
2. each curve must possess a unique tag;
3. each surface must possess a unique tag;
4. each volume must possess a unique tag.

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.

5.1 Geometry commands

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.”

5.1.1 Points

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).

5.1.2 Curves

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.

5.1.3 Surfaces

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.

5.1.4 Volumes

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).

5.1.5 Extrusions

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).

5.1.6 Boolean operations

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.

5.1.7 Transformations

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

5.1.8 Miscellaneous

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.

5.2 Geometry options

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.

6 Mesh module

Gmsh’s mesh module regroups several 1D, 2D and 3D meshing algorithms, all producing grids conforming in the sense of finite elements (see Mesh):

• The 2D unstructured algorithms generate triangles and/or quadrangles (when recombination commands or options are used). The 3D unstructured algorithms generate tetrahedra, or tetrahedra and pyramids (when the boundary mesh contains quadrangles).
• The 2D structured algorithms (transfinite and extrusion) generate triangles by default, but quadrangles can be obtained by using the 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).

6.1 Choosing the right unstructured algorithm

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:

• The “MeshAdapt” algorithm⁷ is based on local mesh modifications. This technique makes use of edge swaps, splits, and collapses: long edges are split, short edges are collapsed, and edges are swapped if a better geometrical configuration is obtained.
• The “Delaunay” algorithm is inspired by the work of the GAMMA team at INRIA⁸. New points are inserted sequentially at the circumcenter of the element that has the largest adimensional circumradius. The mesh is then reconnected using an anisotropic Delaunay criterion.
• The “Frontal-Delaunay” algorithm is inspired by the work of S. Rebay⁹.
• Other experimental algorithms with specific features are also available. In particular, “Frontal-Delaunay for Quads”¹⁰ is a variant of the “Frontal-Delaunay” algorithm aiming at generating right-angle triangles suitable for recombination; and “BAMG”¹¹ allows to generate anisotropic triangulations.

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 split into three separate steps. First, an initial mesh of the union of all the volumes in the model is performed, without inserting points in the volume. The surface mesh is then recovered using H. Si’s boundary recovery algorithm Tetgen/BR. Then a three-dimensional version of the 2D Delaunay algorithm described above is applied to insert points in the volume to respect the mesh size constraints.
• The “Frontal” algorithm uses J. Schoeberl’s Netgen algorithm ¹².
• The “HXT” algorithm¹³ is a new efficient and parallel reimplementaton of the Delaunay algorithm.
• Other experimental algorithms with specific features are also available. In particular, “MMG3D”¹⁴ allows to generate anisotropic tetrahedralizations.

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:

• 1D and 2D meshing is parallelized using a coarse-grained approach, i.e. curves (resp. surfaces) are each meshed sequentially, but several curves (resp. surfaces) can be meshed at the same time.
• 3D meshing using HXT is parallelized using a fine-grained approach, i.e. the actual meshing procedure for a single volume is done is 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).

6.2 Elementary entities vs. physical groups

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.

6.3 Mesh commands

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).

6.3.1 Specifying mesh element sizes

There are several ways to specify the size of the mesh elements for a given geometry:

1. First, if the two options 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.
2. Second, if 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.
3. Next, you can specify a general background mesh size, expressed as a combination of so-called mesh size fields:
   • The Box field specifies the size of the elements inside and outside of a parallelepipedic region.
   • The Distance field specifies the size of the mesh according to the distance to some model entities.
   • The MathEval field specifies the size of the mesh using an explicit mathematical function.
   • The 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.)
   • The 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

6.3.2 Structured grids

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.

6.3.3 Miscellaneous

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.

6.4 Mesh options

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.

7 Solver module

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.

8 Post-processing module

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:

• in a ‘2D space’ plot, the scalar points are taken in the same order as they are defined in the post-processing view: the abscissa of the 2D graph is the curvilinear abscissa of the curve defined by the point series, and only one curve is drawn using the values associated with the points. If several time steps are available, each time step generates a new curve;
• in a ‘2D time’ plot, one curve is drawn for each scalar point in the view and the abscissa is the time step.

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.

8.1 Post-processing commands

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,
• etc.

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}
};

8.2 Post-processing plugins

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