Version: 6.6.0
Constructing meshes

Construction of a mesh on some geometry consists of:

Mesh can be computed using your own meshing algorithms written in Python.

## Creation of a mesh object

To construct a mesh:

1. Select a geometrical object for meshing.
2. In the Mesh menu select Create Mesh or click "Create Mesh" button in the toolbar.

"Create Mesh" button

The following dialog box will appear:

3. Apply meshing algorithms and hypotheses which will be used at computation of this mesh.

"Create mesh" dialog box contains several tab pages titled 3D, 2D, 1D and 0D. The title of each page reflects the dimension of the CAD model (geometry) the algorithms listed on this page affect. For example, 3D page lists the algorithms that affect 3D geometrical objects (solids).

Note:
• Some page(s) can be disabled if the source geometrical object does not include shapes (sub-shapes) of the corresponding dimension(s). For example, if the input object is a geometrical face, 3D page is disabled.
• Some algorithms affect the geometry of several dimensions, i.e. "1D-2D" or "1D-2D-3D". If such an algorithm is selected by the user, the dialog box pages related to the corresponding lower level dimensions are disabled.
• 0D page does not refer to the 0D elements, but to 0D geometry (vertices). Mesh module does not provide algorithms that produce 0D elements. Currently 0D page provides only one algorithm "Segments around vertex" that allows specyfying the required size of mesh edges about the selected vertex (or vertices).

For example, you need to mesh a 3D object.

First, type the name of your mesh in the Name box, by default, it is "Mesh_1". Then select the geometrical object you wish to mesh in the Object Browser and click "Select" button near Geometry field (if the name of the object has not yet appeared in Geometry field).

"Select" button

Now you can define 3D Algorithm and 3D Hypotheses, which will be applied to the solids of your geometrical object. Click the "Add Hypothesis" button to add a hypothesis.

Click the "Edit Hypothesis" button to change the values for the current hypothesis.

"Edit Hypothesis" button

Most standard 2D and 3D algorithms can work without hypotheses using some default parameters. The use of additional hypotheses is optional (i.e. you may leave "None" in this box).

Proceed in the same way with 2D and 1D Algorithms and Hypotheses that will be used to mesh faces and edges of your geometry. (Note that any object has edges, even if their existence is not apparent, for example, a sphere has 4 edges). Note that the choice of hypotheses and lower dimension algorithms depends on the higher dimension algorithm.

Some algorithms generate mesh of several dimensions, while others produce mesh of only one dimension. In the latter case there must be one Algorithm and zero or several Hypotheses for each dimension of your object, otherwise you will not get any mesh at all. Of course, if you wish to mesh a face, which is a 2D object, you do not need to define a 3D Algorithm and Hypotheses.

In the Object Browser the structure of the new mesh will be displayed as follows:

It contains:

• a reference to the geometrical object on the basis of which the mesh has been constructed;
• Applied hypotheses folder containing the references to the hypotheses applied at the construction of the mesh;
• Applied algorithms folder containing the references to the algorithms applied at the construction of the mesh.

There is an alternative way to assign Algorithms and Hypotheses by clicking Assign a set of hypotheses button and selecting among pre-defined sets of hypotheses. In addition to the standard sets of hypotheses, it is possible to create custom sets by editing CustomMeshers.xml file located in the home directory. CustomMeshers.xml file must describe sets of hypotheses in the same way as \${SMESH_ROOT_DIR}/share/salome/resources/smesh/StdMeshers.xml file does (sets of hypotheses are enclosed between <hypotheses-set-group> tags).

List of sets of hypotheses. Tag [custom] is automatically added to the sets defined by the user

Consider trying a sample script for construction of a mesh from our TUI Scripts section.

## Evaluating mesh size

After the mesh object is created and all hypotheses are assigned and before Compute operation, it is possible to calculate the eventual mesh size. For this, select the mesh in the Object Browser and from the Mesh menu select Evaluate. The result of evaluation will be displayed in the following information box:

## Previewing the mesh

Before the mesh computation, it is also possible to see the mesh preview.

For this, select the mesh in the Object Browser. From the Mesh menu select Preview or click "Preview" button in the toolbar or activate "Preview" item from the pop-up menu.

"Preview" button

Select 1D mesh or 2D mesh preview mode in the Preview dialog.

1D mesh preview shows nodes computed on geometry edges

2D mesh preview shows edge mesh elements, computed on geometry faces

Compute button computes the whole mesh.

When the Preview dialog is closed, the question about the storage of temporarily created mesh elements appears:

These elements can be kept in the mesh.

## Changing submesh priority

If the mesh contains concurrent submeshes, it is possible to change the priority of their computation, i.e. to change the priority of applying algorithms to the shared sub-shapes of the Mesh shape.

To change submesh priority:

Choose "Change submesh priority" from the Mesh menu or a pop-up menu. The opened dialog shows a list of submeshes in the order of their priority.

There is an example of submesh order modifications taking a Mesh created on a Box shape. The main Mesh object:

• 1D Wire discretisation with Number of Segments=20
• 2D Triangle (Mefisto) with HypothesisMax Element Area

The first submesh object Submesh_1 created on Face_1 is:

• 1D Wire discretisation with Number of Segments=4
• 2D Triangle (Mefisto) with Hypothesis MaxElementArea=1200

The second submesh object Submesh_2 created on Face_2 is:

• 1D Wire discretisation with Number of Segments=8
• 2D Triangle (Mefisto) with Hypothesis MaxElementArea=1200

And the last submesh object Submesh_3 created on Face_3 is:

• 1D Wire discretisation with Number of Segments=12
• 2D Triangle (Mefisto) with Hypothesis MaxElementArea=1200

The sub-meshes become concurrent if they share sub-shapes that can be meshed with different algorithms (or different hypotheses). In the example, we have three submeshes with concurrent algorithms, because they have different hypotheses.

The first mesh computation is made with:

"Mesh order SubMesh_1, SubMesh_2, SubMesh_3"

"Result mesh with order SubMesh_1, SubMesh_2, SubMesh_3 "

The next mesh computation is made with:

"Mesh order SubMesh_2, SubMesh_1, SubMesh_3"

"Result mesh with order SubMesh_2, SubMesh_1, SubMesh_3 "

And the last mesh computation is made with:

"Mesh order SubMesh_3, SubMesh_2, SubMesh_1"

"Result mesh with order SubMesh_3, SubMesh_2, SubMesh_1 "

As we can see, each mesh computation has a different number of result elements and a different mesh discretisation on the shared edges (the edges that are shared between Face_1, Face_2 and Face_3)

Additionally, submesh priority (the order of applied algorithms) can be modified not only in a separate dialog box, but also in the Preview. This helps to preview different mesh results, modifying the order of submeshes.

"Preview with submesh priority list box"

If there are no concurrent submeshes under the Mesh object, the user will see the following information.

"No concurrent submeshes detected"

## Computing the mesh

It is equally possible to skip the Evaluation and the Preview and to Compute the mesh after the hypotheses are assigned. For this, select your mesh in the Object Browser. From the Mesh menu select Compute or click "Compute" button of the toolbar.

"Compute" button

The Mesh Computation information box appears.

If the mesh computation failed, the information about the cause of the failure is provided.

After you select the error, Show Sub-shape button allows visualizing in magenta the geometrical entity that causes it.

3D algorithm failed to compute mesh on a box shown using Show Sub-shape button

Note:
Mesh Computation Information box does not appear if you set "Mesh computation/Show a computation result notification" preference to the "Never" value. This option gives the possibility to control mesh computation reporting. There are the following possibilities: always show the information box, show only if an error occurs or never. By default, the information box is always shown after mesh computation operation.

Publish Sub-shape button publishes the sub-shape, whose meshing has failed, in GEOM component as a child of the mesh geometry, which allows analyzing the problem geometry and creating a submesh on it in order to locally tune the hypotheses.

If the failure is caused by an invalid input mesh and the algorithm has found which mesh entities are bad, Show bad Mesh button appears in the dialog. Clicked, it shows the bad mesh entities in the Viewer in magenta. Sometimes the shown mesh entities are too small or/and hidden by other mesh elements. They can be seen after switching the mesh to Wireframe visualization mode or switching off the visualization of faces and volumes (if any).

Too close nodes causing meshing failure are shown in magenta using Show bad Mesh button

## "Use existing edges" and "Use existing faces" algorithms

It is possible to create a 1D or a 2D mesh in a python script (using AddNode, AddEdge and AddFace commands) and then use such sub-meshes in the construction of a 2D or a 3D mesh. For this, there exist two algorithms: Use existing edges and Use existing faces. For example, you want to use standard algorithms to generate 1D and 3D meshes and to create 2D mesh by your python code. Then you

• create a mesh object, assign a 1D algorithm,
• invoke Compute command, which computes a 1D mesh,
• assign Use existing faces and a 3D algorithm,
• run your python code, which creates a 2D mesh,
• invoke Compute command, which computes a 3D mesh.

Consider trying a sample script demonstrating the usage of Use existing faces algorithm for construction of a 2D mesh using Python commands.

Mesh computed by the sample script shown in a Shrink mode.