Create Tetra Mesh with the Tetramesh Process Manager

1. From the menu bar, click Mesh > Create > TetraMesh Process > Create New.
2. In the Create New Session dialog, enter a session name and location where the template and related files will be saved and click Create.
   The Process Manager browser and panel open.

1. Select geometry.

   To import	Do this
   Geometry	For Import Type, select Geometry. For File Type, select the type of geometry to import. In the Import Filename field, navigate to the desired file. To automatically save an imported CAD file as an HyperMesh file after the import completes, select the Save HM File After Import checkbox. In the Scale Factor field, enter a scale factor if the imported model is in a spatial scale other than what you want to work with. This feature can also be used to convert the model's measurements between metric and English units, for example. Note: Only spatial units are affected, mass and similar qualities are not. For Cleanup tol, choose a method to perform cleanup on imported geometry. Choose Automatic to use the global cleanup tolerance specified on the Options panel, Geometry subpanel. Choose Manual to enter your own tolerance. To move all entities marked as blank to a special component, select the Import blanked (no show) components checkbox. By default, the translator ignores all of the blank flags in the file.
   HyperModel Model	For Import Type, select HM Model. In the Import Filename field, navigate to the desired file.

2. Click Import.
3. Click Next.

1. Cleanup geometry.

   To cleanup geometry by	Do this
   Equivalencing free edges	Click the Free Edges tab. In the Tolerance field, enter the maximum distance across which surfaces can be made equivalent. Surfaces with a gap between them greater than this value will not be made equivalent. Click Equivalence. Edges and other features that fall within the tolerance value of each other are combined.
   Displaying free edges by edge type	Click the Edge Tools tab. Select the checkboxes (Free Edges / T-junctions) for the edge types to display. Adjust display. Click Isolate to display only the surfaces attached to the selected edge types. Click Display All to remove the mask and view all surfaces.
   Create filler surfaces	Click the Edge Tools tab. Click Create to generate filler surfaces for all the free edge loops. This functionality helps to eliminate issues caused from missing surfaces by creating the closed volumes necessary for tetrameshing.

2. Click either Accept or Next to continue.

Isolate holes based on diameter ranges. Isolating and meshing holes separately from other geometry features is a very important step during tetra meshing; failing to do so can drastically affect the overall mesh quality. You may also wish to use this step even when there are no specific meshing requirements for holes just to organize your model.

1. Click + to add additional rows to the table if you require multiple sets of hole criteria.
2. In the D< field, enter diameter values to consider when selecting holes.
   Holes with diameters less than the value you specify will be automatically selected. If you add multiple lines to the table, HyperMesh generates non-overlapping ranges from them.

   Tip: If you have no specific requirements for hole meshing, you can use a single diameter value that is larger than the largest holes in the model, in order to select all of the holes.
3. In the Num Circumference Elems field, enter the number of elements to place around the circumference of any holes of the specified diameter range.
   Higher numbers result in a smoother mesh that better approximates a hole's shape and curvature, but could impact tetramesh quality if they result in smaller elements around the hole's edges than the enforced element size for other surfaces.

   Tip: If you have no specific requirements for hole meshing, it is recommend that you use at least 6 elements for each hole's circumference.
4. In the Longitudinal Elem Size field, enter the desired element size in the longitudinal direction.
   Longitudinal direction is the direction traveled along the depth of the hole.

   Tip: If you have no specific requirements for hole meshing, it is best to use the same element size as the rest of the model.
5. Click Auto Organize to automatically organize the holes into separate components based on the input parameters, diameter, and so on.

   One component will be created for each row in the table, and the holes are placed into the components that their diameter and other criteria match. The model holes, and corresponding table rows, are color-coded according to the component that they have been sorted into.

   Clicking one of these buttons selects the entire row, making it the "active" row. To deselect an active row, click the colorless button at the very top-left corner of the table (the one in the header row along with the column names).

   
   
   Figure 1.

6. Click Organize to manually organize any holes that were missed by Auto Organize into components using the Organize panel.
7. Click either Accept or Next to continue.

1. From the Mesh Type column, select the mesh type to use when meshing the holes.
   There are two meshing options available: R-tria regular and R-tria union jack.

   Figure 2. R-tria regular	Figure 3. R-tria union jack

2. Mesh holes.

   Each row has a color button on its left which corresponds to the component holding hole surfaces. Clicking one of these buttons selects the entire row, making it the "active" row. To deselect an active row, click the colorless button at the very top-left corner of the table (the one in the header row along with the column names).

   • To mesh a single group of hole, select it's corresponding row and click Mesh.
   • To mesh all of the holes simultaneously, click Mesh All.

   
   
   Figure 4.

3. Click either Accept or Next to continue.

Organize and cleanup user defined features such as water jackets, inlets, outlets and contact surfaces.

1. Create a feature by clicking +.
2. In the dialog that opens, enter a name for the feature and click OK.
3. Use the surfs selector to select the surfaces associated with the feature, which will be added to a new component.
   When selecting surfaces, surfaces are added "by face" to the selection to allow all of the surfaces associated with the same face in the model to be added simultaneously.
4. Click proceed to finish adding surfaces to the component.

   Features are sorted into color-coded components and the corresponding table rows are colored to match.

5. Select a feature's corresponding row to make it active, then click Auto Cleanup.
6. In the Autocleanup panel, perform automated geometry cleanup operations on the geometry contained in the selected component.
7. Click either Accept or Next to continue.

Defeature fillets, and replace the rounded corner where two lines come together with a point. Tangents are calculated at the beginning and at the end of each fillet, then those tangents are intersected to create a corner.

1. Use the Components selector to select the components that contain the fillets that require cleanup.
2. In the Min Radius field, enter a minimum fillet radius to cleanup.

   Any fillets in the model with radii of less than this value will be ignored, while fillets with radii greater than this will be cleaned up (removed so that the relevant lines meet at a sharp corner.)

3. In the Max Radius field, enter a maximum fillet radius to cleanup.

   Fillets with radii greater than this value will be ignored and remain.

4. To suppress such edges after the fillet removal process, select the Suppress fillet tangent edges checkbox.
   Because fillets are removed by generating tangent lines to replace them, these lines often result in extra edges in model geometry.

   Figure 5. Suppress Fillet Tangent Edges On	Figure 6. Suppress Fillet Tangent Edges Off

5. Click Cleanup.

   The fillet midline split routine is executed based on what you have specified for the radius range and tangent suppression.

6. Click either Accept or Next to continue.

1. For Mesh Type, select the type of elements used to generate the mesh for each feature.
2. In the Elem Size field, enter the element size used to generate the mesh for each feature.
3. Create mesh.
   • To create mesh for the selected/active row, click Mesh.
   • To create mesh for all rows, click Mesh All.
4. Click either Accept or Next to continue.

Organize and clean up all remaining global surfaces, that is, surfaces that were not already covered by holes and user-defined features.

1. In the Min Element Size field, enter a minimum element size for all such components to prevent the autocleanup process from accidentally suppressing very small surfaces. Smaller values result in more aggressive geometry cleanup, but could potentially result in loss of some features.
2. Optional: Click Organize to organize remaining surfaces into appropriate components using the Organize panel.
3. Click Auto Cleanup.
   The Autocleanup panel opens, which can be used to clean all remaining surfaces.
4. Click either Accept or Next to continue.

Mesh all remaining global surfaces, that is, surfaces that were not already covered by holes and user-defined features.

1. In the Element Size field, enter the element size to use when meshing.
2. For Mesh Type, choose the type of element to use when meshing.
3. Click Mesh.
   A mesh is created using the specified element size and type on all remaining "global" geometry.

   Note:

   If you do not like the results, click Delete Mesh to remove mesh from all such geometry, without affecting the specific items already meshed in previous stages, such as holes or user-defined features.

4. Click either Accept or Next to continue.

Optimize the quality of the elements created during each of the previous meshing stages.

• Perform automatic cleanup.
  Note:

  The nodes of features, such as ridges, will not be preserved if their angle is less than the specified minimum angle. In addition, element quality requirements may override feature angle preservation regardless of the angle specified.

  1. Click the Auto tab.
  2. Use the Components selector to select the components that contain the elements to cleanup.
  3. In the Min Size field, enter the minimum size that is acceptable for any given elements.
  4. In the Max Feature Angle field, enter the maximum feature angle to preserve.

     Figure 7. Minimum Feature Angle (Low Value)	Figure 8. Minimum Feature Angle (High Value)

  5. In the Normals Angle field, enter the maximum allowable angle between the normals of adjacent elements.
     When possible, adjacent elements whose normals exceed this angle will be split into multiple smaller elements with less-extreme normal angles.
  6. Click AutoCleanup.
  7. Click either Accept or Next to continue.
  The mesh is examined within each component individually, removing elements of poor quality and stitching the mesh together to fill the resulting gaps. Cleaning up the mesh on a per-component basis prevents mesh overlap between adjacent surfaces that belong to different components.

  Figure 9. Before Element Cleanup. Notice the "sliver" elements along midline.	Figure 10. After Element Cleanup. Notice the small, sliver elements are removed.

• Perform manual cleanup.
  1. Click the Manual tab.
  2. Choose the type of edges to find.
     • Choose Free to find edges which are associated with only 1 surface.
     • Choose T-Connections to edges which are associated with three edges.
  3. Click Find to find edges.
  4. In the Tolerance field, enter the tolerance to use when identifying nodes associated with free edges and try to stitch them, leaving nodes outside the tolerance unchanged.
  5. Click Fix to fix free edegs.
  6. Click Display Normals to open the Normals panel, which can then be used to review normals.
  7. Click either Accept or Next to continue.

Generate the 3D mesh from the existing surface meshes.