Polyhedral meshes contain polyhedral cells. An advantage that polyhedral meshes have shown relative to tetrahedral or hybrid meshes is the lower overall cell count, almost 3-5 times lower for unstructured meshes than the original cell count. Since the polyhedral mesh has a lower cell count than the equivalent original tetrahedral mesh, solution convergence will generally be faster, possibly saving some computational expense.
Polyhedral meshes can be generated using the object-based volume meshing approach. The starting point is a valid surface mesh (see Surface Mesh Processes).
Prerequisites for generating a polyhedral mesh include:
A valid surface mesh must be a triangular mesh of good quality.
Surface triangulation size should not exceed material thickness.
The aspect ratio of prisms should be less than 50.
Note: The polyhedral meshing process changes triangle faces in the surface mesh to hexagonal faces. Once the polyhedral mesh exists, you cannot regenerate the volume mesh unless you first select the option. When you select , the current object face zones and cell zones are deleted. You can then begin the volume meshing process again using the original valid surface mesh as the starting point. See Generating the Volume Mesh for more information about .
The process followed and steps required to generate the polyhedral mesh are explained.
The Auto Mesh dialog box contains options for setting up and generating a polyhedral mesh from a valid surface mesh for all computed volumetric regions of the mesh object.
If enabled, the prism mesh is generated based on the scoped prism settings specified. Polyhedral meshing does not support zone-specific prisms.
The polyhedral meshing process starts by generating a tetrahedral mesh in two stages: initialization and refinement.
The automatic initialization procedure includes the following steps:
Merging free nodes.
Deleting unused nodes.
Improving the surface mesh based on polyhedra-driven criteria.
Initializing the mesh.
Generating and separating cell regions.
The cell zones are then associated with the regions and the cell zone type will be applied. Dead cell zones will be deleted.
The refinement procedure includes the following steps:
Inserting nodes for refining the mesh.
Two stages of tet mesh improvement.
The polyhedral mesh is created as a dual of the tetrahedral mesh, such that the vertex of the mesh-element (tetrahedron) is close to the center of the solver-element (polyhedron). Tessellations are created for the boundary and cell zones. When prism mesh is generated, the dual is used directly, meaning the layering structure of the mesh is maintained.
The polyhedral mesh is improved by operations like merging short edges and splitting cells. Concave cells, concave boundary faces, and stair-stepped poly cells are split to improve quality. The quality is further improved by smoothing.
The best quality measures for polyhedral meshing are squish and ortho skew. If you select squish or ortho skew, skewness evaluations during smoothing will be supplemented with additional internal measures. If you select a quality measure other than squish or ortho skew, mesh generation will use an internal variant of squish because it provides some direct control over the convexity of the cell.
The Auto Mesh dialog box contains options to control the polyhedral volume mesh generation.
You can generate the poly mesh as follows:
Open the Auto Mesh dialog box from the context-sensitive menu available by right-clicking on any mesh object or its Volumetric Regions or Cell Zones branch in the tree.
You can also use the > menu item to open the Auto Mesh dialog box.
Ensure that the mesh object is selected in the Object drop-down list.
Note: If you open the Auto Mesh dialog box from the context-sensitive menu in the tree, the Mesh Object to which the cell zones or volumetric regions belong is automatically selected.
Enable/disable the Keep Solid Cell Zones option, as appropriate.
Select the appropriate option in the Grow Prisms drop-down list in the Boundary Layer Mesh group box.
Retain the default selection of none if you do not need to grow prism layers for the current meshing approach.
Select scoped if you want to specify object-based prism controls. Click to open the Scoped Prisms dialog box and define the prism controls for the mesh object. Refer to Prism Meshing Options for Scoped Prisms for details.
Tip: You can save your scoped prism controls to a file (*.pzmcontrol) for use in batch mode, or read in a previously saved scoped prism file.
Note:Poly meshing does not support zone-specific prisms.
Stair-stepping will occur in regions of transition between the prism layers and the adjacent tets.
Set the Poly mesh parameters.
Select the Poly option from the Volume Fill list and set the following Volume Fill Options.
Select the appropriate option for Cell Sizing.
Size Field specifies that the cell size is determined based on the current size-field.
Geometric specifies that the cell size in the interior of the domain is obtained by a geometric growth from the closest boundary according to the growth rate specified.
Set the Growth Rate required.
Specify the Max Cell Length. Click to compute the maximum cell size based on the mesh object.
Note: You can also set these parameters in the Poly dialog box.
Click the Set... button to open the Poly dialog box.
Select the options in the Options group box.
The Merge Free Nodes, Delete Unused Nodes, and Improve Poly Mesh options are enabled by default. You can also include improving the surface mesh by enabling the Improve Surface Mesh option.
Specify an appropriate value for Feature Angle. This sets the threshold for preserving features. The default setting is 30 degrees.
Select the appropriate cell zone type from the Non-Fluid Type list in the Poly Zones group box.
Note: Dead cell zones will be automatically deleted after the mesh is initialized.
When the initial mesh is generated, all the cells are grouped into contiguous zones separated by boundaries. The mesh is considered to contain a single fluid zone and one or more dead regions. The zone just inside the outer boundary is set to be active and is labeled a fluid zone. All other non-fluid zones will be inactive. Only active zones will be considered for refinement during the mesh generation process.
Note: Volume region type is used to determine the cell zone type.
You can refine different groups of zones using different refinement parameters for each group by toggling the zones between active and inactive. If however, you need to use the same refinement parameters for all the zones, you can change the specification of Non-Fluid Type to a type other than dead (for example, solid). When the Non-Fluid Type is set to a type other than dead, all the zones will be activated after initialization. Hence, you can set the appropriate refinement parameters without setting all the zones to be active.
In most cases, the default node spacing threshold should be acceptable. If you want to change it, click Controls to open the Poly Init Controls dialog box where you can modify the value.
Set poly cell growth parameters using the options in the Cell Size group box. Specify appropriate values for Max Cell Volume and Growth Rate. You can use the button to determine the maximum cell size based on the size field.
Ensure that cells in the interior are not larger than the size required by selecting the appropriate option in the Cell Sizing list:
- geometric
specifies that the cell size in the interior of the domain is obtained by a geometric growth from the closest boundary according to the growth rate specified.
- size-field
specifies that the cell size is determined based on the current size-field.
Click the button to access the Tet Refinement Region dialog box, where you can setup and activate local tetrahedral refinement regions. These regions are used during the initial tetrahedral mesh generation; they are not directly applicable to the poly mesh. The number of activated regions will be reported in the Message field.
Return to the Auto Mesh dialog box and enable or disable additional Options as desired.
Enable Merge Cell Zones within Regions to create a single cell zone within a region, or disable to keep the cell zones separate.
Click in the Auto Mesh dialog box.
Examine the following after completing the automatic mesh generation process:
The mesh size with the Report Mesh Size dialog box (see also Determining Mesh Statistics).
The prism layer cell quality distribution (see Determining Boundary Cell Quality).
The polyhedral cell quality reports (see Determining Volume Mesh Quality).
Note: The quality measure will be set to Inverse Orthogonal Quality after the polyhedral mesh is generated.
Node weights for node-based gradients are enabled by default for poly meshes generated in Fluent Meshing. This setting can improve the accuracy of the displayed results near wall edges when you are displaying contours on a native 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.