Generating the Volume Mesh

After assigning geometry parts to regions, you can proceed to define and generate the volume mesh using mesh operations. Mesh operations are defined within the Geometry > Operations node.

Several steps are involved in defining and generating a volume mesh. In this tutorial, you can proceed immediately to define an automated mesh operation and choose the meshers. Other cases can require preliminary operations such as those for transforming parts or modifying them using Boolean operations.

Within the automated mesh operation, you select different meshers for the generation of the surface mesh, the volume mesh, and the prism layers that are created at the wall boundaries of the computational domain. The selected meshers within this automated mesh operation apply to one or more selected geometry parts. You can create several automated mesh operations containing different meshers and mesh settings. Here, you create only one automated mesh operation that applies to one geometry part.

To select the meshers:

  1. Right-click Geometry > Operations and select New > Mesh > Automated Mesh.


  2. In the Create Automated Mesh Operation dialog:
    1. In the top part of the dialog, from the Parts list, select subdomain-1 .
    2. In the lower part of the dialog, within Select Meshers, select the following meshers in order:
      Group Mesher
      Surface Meshers Surface Remesher
      Core Volume Meshers Polyhedral Mesher
      Optional Boundary Layer Meshers Prism Layer Mesher
      The final dialog looks as shown below:

    3. Click OK.
  3. Expand the Operations > Automated Mesh > Meshers node.


Generating a mesh often requires several iterations to achieve the desired density and distribution of cells. In this tutorial, to avoid repetition, you specify the global mesh settings and then make some further customizations.

To specify the global mesh settings:

  1. Within the Geometry > Operations > Automated Mesh node, right-click the Default Controls node and select Edit....
  2. In the Default Controls dialog, click Expand/Contract Tree, then set the following properties:
    Node Property Setting
    Base Size Base Size 0.01 m
    Prism Layer Controls Numbers of Prism Layers 5
    Prism Layer Total Thickness Percentage of Base 20
    • After setting the properties, click Close.
    With this base size, approximately 8 cells are created across the width of the region.
Before generating the mesh, you make two customizations to the mesh settings:
  1. By default, the prism layers are generated on the inner and the slip walls by default. However, a fluid boundary layer does not form on slip walls and prism layers are not required. Using a surface control, you can customize the prism mesh settings on that boundary to disable the prism layer generation.
  2. To provide higher mesh resolution around the blunt body itself, apply a second surface control with a smaller target surface size.
  1. To disable the prism layer generation on the slip wall:
    1. Right-click the Geometry > Operations > Automated Mesh > Custom Controls node and select New > Surface Control.
    2. Right-click the Custom Controls > Surface Control node and select Edit.
    3. Set the following properties:
      Node Property Setting
      Surface Control Part Surfaces Slip_wall
      Controls > Prism Layers Prism Layers Disable
  2. To reduce the mesh size on the blunt body surface:
    1. Right-click the Automated Mesh > Custom Controls node and select New > Surface Control.
    2. Right-click the Custom Controls > Surface Control 2 node and select Edit.
    3. Set the following properties:
      Node Property Setting
      Surface Control 2 Part Surfaces Inner_wall
      Controls > Target Surface Size Target Surface Size Custom
      Controls > Minimum Surface Size Minimum Surface Size Custom
      Values > Target Surface Size Size Type Absolute
      Absolute Size 0.001 m
      Values > Minimum Surface Size Size Type Absolute
      Absolute Size 1.0e-4 m
Now that all mesh settings are defined, you can generate the mesh.
  1. Click (Generate Volume Mesh) in the toolbar or select Generate Volume Mesh in the Mesh menu.

    The run and progress of the meshers are displayed in the Output window.

  2. To display the volume mesh, from the Vis toolbar, click (Create/Open Scenes) and select Mesh.
  3. In the graphics window, zoom in to see the mesh around the leading corner of the blunt body.