11.1. Volume Mesh Process

When the conformal, connected surface mesh is ready, use the model tree to navigate the volume meshing workflow as follows:

  1. Set up Volumetric Regions.

    Volumetric regions are finite, contiguous domains ready to receive a volume mesh. You use the Compute menu option to initialize the volumetric regions within a mesh object. If you perform operations such as merging or deleting, you should Validate the regions before computing the volume mesh. The Update option will recompute existing volumetric regions while preserving names and types.

    Tools to compute, update and validate the volumetric regions, as well as tools to modify selected regions, are accessible via the context-sensitive menus. For a full description of available operations, see Volumetric Region Management.

  2. Fill the volumetric regions collectively or individually, as appropriate.

    1. Right-click on any individual volumetric region and you can access menus to setup Scoped Prism, Tet, or Hexcore volume meshing parameters, as appropriate. Descriptions of meshing parameters are found in Prism Meshing Options for Scoped Prisms, Generating Tetrahedral Meshes, and Generating the Hexcore Mesh.

      After setting mesh parameters, you can compute the mesh in an individual volumetric region using the Auto Fill Volume option. See Meshing Regions Selectively Using Auto Fill Volume.

    2. To apply meshing parameters and compute the volume mesh collectively for all volumetric regions of the selected object(s), use the Auto Mesh option in the Volumetric Regions context menu. See Meshing All Regions Collectively Using Auto Mesh.

      You can also access the Auto Mesh option from the object level context menu, and access the scoped prism option directly using Setup Scoped Prisms... from the Volumetric Regions menu.

  3. Examine the volume mesh and verify the mesh quality.

    1. The computed volume mesh is placed into Cell Zones. You can use the context menus to draw the cell zones individually or collectively to examine the mesh. Cell zones may be merged or deleted if necessary. Volumetric regions are not affected if cell zones are deleted. Refer to Cell Zone Options.

    2. Improve the mesh quality using the Auto Node Move tool, if needed. See Moving Nodes.

When you are satisfied with the quality of the volume mesh, prepare the mesh for transfer to solution mode. Right click on Model at the top of the tree and select Prepare for Solve from the context menu. Operations such as deleting dead zones, deleting geometry objects, deleting edge zones, removing face/cell zone name prefixes and/or suffixes, and deleting unused faces and nodes are performed during this operation.


Important:  In object-based workflows, merging cell zones requires that they be in the same volumetric region.

To merge cell zones that cannot be in the same volumetric region because they are not contiguous, you will need to first delete the object(s) only, and then use the Manage Cell Zones dialog box.



Note:  When you generate a poly mesh, node weights for node-based gradients are enabled by default. For postprocessing, this setting can improve the accuracy of the displayed results near wall edges when you are displaying contours on the poly mesh. When you transfer the poly mesh to solution mode, a message will notify you that this interpolation is enabled. You can disable it by setting the /display/set/nodewt-based-interp? command to no.



Release 18.2 - © ANSYS, Inc. All rights reserved.