Creating Octree 3D Mesh Parts

This task shows you how to create a 3D mesh using Octree tetrahedron elements.

This command is available both in the Generative Structural Analysis workbench and in the Advanced Meshing Tools workbench. Options available in the Octree tetrahedron mesher are different depending on the products you have installed:

• Generative Part Structural Analysis (GPS) or FEM Surface (FMS) products
• FEM Solid (FMD) product.

Generative Part Structural Analysis (GPS) or FEM Surface (FMS)

In this configuration, the dialog box allowing you to define Octree 3D mesh parts contains only two tabs either in the Generative Structural Analysis workbench or in the Advanced Meshing Tools workbench.

1. Click Octree Tetrahedron Mesher (in the Model Manager toolbar for the Generative Structural Analysis workbench or the the Meshing Methods toolbar for the Advanced Meshing Tools workbench).

2. Select the part you want to mesh.

   In this particular case, select PartBody. You can only select 3D geometries belonging to the default PartBody. The OCTREE Tetrahedron Mesh dialog box appears. Global tab: lets you change global parameters. To know more, refer to the global tab description. Local tab: lets you create local parameters. To know more, refer to the local tab description.

3. Enter the desired options in the OCTREE Tetrahedron Mesh dialog box.

   In this case, enter 24mm as Size value.

4. Click OK in the OCTREE Tetrahedron Mesh dialog box.

   The new mesh part has been created manually and the specification tree is updated. If you rename the part that is the support of a mesh part, the mesh part is also renamed but this change is not dynamically displayed in the specification tree. You must collapse and expand again the Nodes and Elements node or the Finite Element Model node of the specification tree.

3D mesh can be deleted and/or added to parts manually.

FEM Solid (FMD)

In this configuration, the dialog box allowing you to define Octree 3D mesh parts contains four tabs either in the Generative Structural Analysis workbench or in the Advanced Meshing Tools workbench.

1. Click Octree Tetrahedron Mesher (in the Model Manager toolbar for the Generative Structural Analysis workbench or the the Meshing Methods toolbar for the Advanced Meshing Tools workbench).

2. Select the solid you want to mesh.

   You can only select 3D geometries belonging to the default PartBody. The OCTREE Tetrahedron Mesh dialog box appears. Global tab:   Size: lets you choose the size of the mesh elements. To know more about the Element Type you have to choose in the OCTREE Tetrahedron Mesh dialog box, refer to Linear Tetrahedron and Parabolic Tetrahedron in the Finite Element Reference Guide. Absolute sag: maximal gap between the mesh and the geometry.   Proportional sag: is the ratio between the local absolute sag and the local mesh edge length. Proportional sag value= (local Absolute sag value) / (local mesh edge length value) Note that Absolute sag and Proportional sag could modify the local mesh edge length value. You can use both Absolute sag and Proportional sag, the most constraining of the two values will be used. Element type: lets you choose the type of element you want (Linear or Parabolic). Local tab: You can also add local meshing parameters such as sag, size or distribution to the part. To add a local specification, select the desired Available specs, and then click the Add button. A different dialog box appears according to the option you have selected. Local size: you can modify the Name, Support and Value. Local sag: you can modify the Name, Support and Value. Edges distribution: lets you distribute local nodes on a edge. To add an edge distribution: Select the Edges distribution option and click Add. The Edges Distribution dialog box appears. Select the edge on which you want to assign nodes (Supports) as well as the Number of Edges to be created. Edges Distribution.1 appears in the specification tree as well as the nodes on the selected edge. Click OK in the Edges Distribution dialog box. Imposed points: lets you select the points that will be taken into account when meshing. In this case, the points you have to select must have been created via Shape Design or Part Design. Only points on curve or points on surface are supported. The points support must be a member of the meshed geometry. To impose points: Select the Local imposed points option and click Add. The Imposed Points dialog box appears. Select from the specification tree the points (Supports) you will impose for OCTREE tetrahedron mesh generation. Click OK in the Imposed Points dialog box. To edit the local specification that has just been created, double-click Imposed Points in the specification tree and modify the desired options in the Imposed Points dialog box that appears. Size Distribution: lets you impose a distribution on a selection of curves by specifying the size. This local specification is used to calculate the nearest number of edges for each support to approximate the specified size. You can select only curves or faces. If you select a face, the distribution is applied to all the boundary curves of the face. If two distribution sizes with different value are applied on the same curve, only the smallest distribution is taken into account. In case of conflict between edge distribution and size distribution, the edge distribution specification is taken into account. This specification has an effect only near the concerning curves. It cannot be used to stabilize mesh inside large faces. To add a size distribution: Select Size distribution and click Add. The Size Distribution dialog box appears. Select curves or faces. In the Value box, enter a size value. Click OK. Quality tab   Criteria: lets you choose a criterion (Shape, Skewness or Strech) to optimize the mesh quality. Intermediate nodes parameters: only available if you have chosen a Parabolic element type in the Global tab. This option lets you choose the position of parabolic tetrahedron intermediate nodes (Jacobian or Warp). The distance (d) between the geometry and the intermediate node is function of Jacobian and Warp values.
   	For more details about mesh quality analysis, refer to  Analyzing Element Quality in the Advanced Meshing Tools User's Guide.
   Others tab: Details simplification: lets you remove small mesh. Geometry size limit: lets you specify the maximum size of the elements to be ignored by the mesher (before meshing). If all the edges of a surface are smaller than the Geometry size limit value, this surface will be ignored by the mesher. Mesh edges suppression: removes small edges (after meshing). Without Mesh edge suppression: With Mesh edge suppression: It may happen that Mesh edge suppression involve constraints violation. Global interior size: lets you specify the maximum interior size of the mesh. If the value of the Global interior size is smaller than the value of the Size, the value of the Size will be reduced to the value of the Global interior size. Global split: lets you generate a mesh with at least two element layers, even in thin material areas. All the mesh edges that satisfy one of the following conditions will be split automatically: A mesh edge on a curve connects two nodes on vertices. A mesh edge on a face connects two nodes on curves or vertices. A mesh edge inside a volume connects two surface nodes. If you select the Global split check box, the mesh quality decreases in areas with small geometry (small edges, thin faces). Min. size for sag specs: lets you specify the minimum size of the mesh refining due to sag specifications. Max. number of attempts: lets you impose a maximum number of attempts, if several attempts are needed to succeed in meshing, in the case of a complex geometry.

3. Select the desired parameters.

   In this particular example, preserve the default parameters.

4. Click Apply.

   The Computation Status dialog box appears and the mesh is generated on the part. For a better visualization, hide the geometry. To do this, right-click the Links Manager.1 object and select Hide/Show. The OCTREE Tetrahedron Mesh.1: Part.1 object appears in the specification tree.

5. Click OK.

6. To edit the Octree tetrahedron mesh, double-click the OCTREE Tetrahedron Mesh.1: Part.1 object in the specification tree.

   The OCTREE Tetrahedron Mesh dialog box reappears.

If you rename the part that is the support of a mesh part, the mesh part is also renamed but this change is not dynamically displayed in the specification tree. You must collapse and expand again the Nodes and Elements node or the Finite Element Model node of the specification tree.