Tetra/Mixed Mesh Type

There are four different Mesh Methods available for Tetra/Mixed Meshing: Robust (Octree), Quick (Delaunay), Smooth (Advancing Front), and Ansys Fluent Meshing. The different options for each mesh method are:

Robust (Octree) Mesh Method

This algorithm ensures refinement of the mesh where necessary (based on entity sizes and the curvature and proximity based refinement settings), but maintains larger elements where possible, according to the ICEM CFD octree algorithm and applied settings (such as tetra ratio). For additional information see The Octree Mesh Method.

Create Prism Layers

generates post inflation prism layers in the tetra volume mesh that is created, according to the prism meshing parameters that are specified under Global Mesh Setup > Prism Meshing Parameters, Part Mesh Setup, Surface Mesh Setup, and/or Curve Mesh Setup.

Create Hexa-Core

generates a hexa-core mesh using a bottom-up meshing approach. It will retain the tri surface or prism mesh, delete the existing tetra mesh, and remesh the volume interior with Cartesian meshing. The tetra elements will be mapped to the tri or prism faces with the Delaunay algorithm.

Input

specifies the geometry that will be used as input for the Volume Mesh.

All: meshes the entire geometry.
Visible: meshes the visible geometry.
Part by Part: meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From File: runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or browse the file manager.
Use Existing Mesh Parts: forces the Octree Tetra mesher to align to the surface mesh of the selected existing mesh parts when the All or Visible option is selected for the input geometry. The Octree tetra mesh will be generated in its normal top down (volume first) method and then be “made conformal” with the existing surface mesh.

Quick (Delaunay) Mesh Method

uses the Delaunay Tetra mesher and a bottom-up meshing approach to generate a mesh. The surface mesh can be an existing mesh or will be created with the parameters defined under Global Mesh Setup > Shell Meshing Parameters or Surface Mesh Setup. The volume mesh will then be generated from this surface mesh. The Delaunay method is robust and fast.

Note: This method works with quads or tris or a combination of both. Quads will use pyramids to transition to the Tetras. The surface mesh can have multiple volumes and have multiple edge elements. However, the Delaunay mesh method requires a closed surface mesh, and cannot tolerate single edges, overlapping elements or duplicate elements. You can run a mesh check ( Edit Mesh > Check Mesh ) before generating the volume mesh. Also, sudden changes in element size, either adjacent or across a narrow volume gap, can cause quality issues or failure.

Create Prism Layers

Create Hexa-Core

The Hexa-Core mesh parameters are specified under Global Mesh Setup > Volume Meshing Parameters > Cartesian Mesh Type > Hexa-Core Mesh Method.

Volume Part Name

allows you to select from the list of existing volume parts, select a part from the screen, or supply a new name. The created mesh will be assigned to this part name.

If you select inherited, the mesher will place the volume element into the same part as an existing material point. For the Delaunay method, the existing material point name will be used, but without its specific location. This option works well for models with only one material point. For more advanced models, such as conjugate heat transfer models or models with sections of porous media, you should enable the Flood fill after completion option (available in the Quick (Delaunay) mesh method options) to use each material point with its location to determine the volume mesh part names for each region.

Note: When the inherited option is selected, the mesher will run the flood fill operation, even if Flood fill after completion is disabled under Volume Meshing Parameters in the Global Mesh Setup.

Input

specifies the geometry that will be used as input for the Volume Mesh.

All Geometry: meshes the entire geometry.
Existing Mesh: allows the mesher to align to the existing mesh.
Part by Part: meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From File: runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or browse the file manager.

Smooth (Advancing Front) Mesh Method

This option will use the Advancing Front Tetra mesher to generate a mesh using a bottom-up meshing approach. The surface mesh will be created with the parameters defined under Global Mesh Setup > Shell Meshing Parameters or Surface Mesh Setup. The volume mesh will then be generated from this surface mesh.

Note: The surface mesh should be one enclosed volume with no single edges, multiple edges, non-manifold vertices, overlapping elements or duplicate elements. Sudden changes in element size, either adjacent to one another or across a narrow volume gap, can cause quality issues or even failure.

The surface mesh must be either tri or quad elements for the Advancing Front mesh method.

The primary advantage of the Advancing Front Method is the ability to generate a smoothly transitioning Tetra mesh, with a volume growth ratio controlled by the Expansion Factor under the Global Mesh Parameters.

Create Prism Layers

Volume Part Name

allows you to select from the list of existing volume parts, select a part from the screen, or supply a new name. The created mesh will be assigned to this part name.

If you select inherited, the mesher will place the volume element into the same part as an existing material point. For this method, the existing material point name will be used, but without its specific location. This option works well for models with only one material point. For more advanced models, such as conjugate heat transfer models or models with sections of porous media, you should enable the Flood fill after completion option (available in the Smooth (Advancing Front) mesh method options) to use each material point with its location to determine the volume mesh part names for each region.

Input

specifies the geometry that will be used as input for the Volume Mesh.

All Geometry: meshes the entire geometry.
Existing Mesh: allows the mesher to align to the existing mesh.
Part by Part: meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From File: runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or browse the file manager.

Fluent Meshing

This option will use Ansys Fluent Meshing technology to create a tetrahedral volume mesh from an existing geometry and/or mesh, with additional options for boundary layer inflation and/or hexa-core volume mesh.

Create Prism Inflation Layers

Enables the prism creation processes and allows you to select an inflation option.

Post Inflation Layers: replaces the tetrahedral mesh near the surfaces with prism layers using the ICEM CFD post inflation algorithm, according to the prism meshing parameters that are specified under Global Mesh Setup > Prism Meshing Parameters, Part Mesh Setup, Surface Mesh Setup, and/or Curve Mesh Setup.
Pre Inflation Layers: creates prism layers from the surface mesh using the Ansys Fluent Meshing pre inflation algorithm before filling with tetrahedral mesh. If no geometry is available to identify prism growth direction, pure tetra meshing will be done without prisms.

Create Fluent Mesh with Hexa-Core

The Delaunay algorithm is used to fill the gap between the hexa core elements and the surrounding shell mesh or prism layer with conformal tetra and pyramid elements.

Run interactive Fluent Meshing

imports the mesh and settings but the journal macros need to be run interactively. Recommended for expert users only.

Volume Part Name

allows you to select from the list of existing volume parts, select a part from the screen, or supply a new name. The created mesh will be assigned to this part name.

If you select inherited, the mesher will place the volume element into the same part as an existing material point. For this method, the existing material point name will be used, but without its specific location. This option works well for models with only one material point. For more advanced models, such as conjugate heat transfer models or models with sections of porous media, you should enable the Flood fill after completion option (available in the Fluent Meshing mesh method options) to use each material point with its location to determine the volume mesh part names for each region.

Frozen volume mesh parts

allows you to select parts that will not be remeshed when using the Fluent Meshing option. This is useful, for example, to preserve one or more meshed regions while remeshing others.

Note:

Parts to be remeshed require a volume mesh. A surface mesh and material point is not sufficient.
If remeshing a tet mesh region next to a frozen hex mesh, the tet mesh will be connected to the hex mesh using pyramids. Inflation layers will connect to the hexas, if possible.

Input

specifies the source data for the volume mesher.

All Geometry

meshes the surfaces according to the global surface mesh setup, then grows the volume mesh from the surface mesh.

Existing Mesh

grows the volume mesh from the existing surface mesh.

If no surface mesh exists, one is created from the existing volume mesh.

Part by Part

meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.

From File

runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or browse the file manager.