HM-3270: Use the Tetramesh Process Manager

In this step you will initiate the process manager.

1. Start a new session in the TetraMesh Process Manager by clicking Mesh > Create > TetraMesh Process > Create New from the menu bar.
2. In the Create New Session dialog, type a name for the session in the New Session Name field.
   Note: Creating a session name and saving the session allows you to stop the process before completion and then load it again at a later time, picking up the process at the point it was left off.
3. In the Working Folder field, navigate to the location of your working directory.
4. Click Create.
   The Process Manager opens in the tab area.

In this step you will import geometry.

1. In the panel area, set Import Type to HM Model.
2. In the Import Filename field, open the file, tetmesh_pm.hm.
3. Click Import.
   The model is imported.

   Note: A green checkmark appears next to the Geometry Import step in the Process Manager tab, which indicates that the step is complete.

In this step you will clean up the geometry.

1. On the Visualization toolbar, select from the list of geometry color modes and click to shade the model's geometry and surface edges.
2. In the panel area, select the Edge Tools tab.
3. Click Isolate.
   HyperMesh isolates the surfaces with free edges on them.

   
   
   Figure 1.

4. Select the Free Edges tab.
5. Click Equivalence.
   All free edges are fixed.

   Note: If this did not correct all free edges, increase the Tolerance value until all free edges are equivalenced.
6. Select the Edge Tools tab.
7. Click Isolate.
   A dialog appears with a message that reads, "No edges found..."

   Note: This confirms that all edges have been fixed.
8. Click Display All.
   The entire model is displayed.
9. Click Accept.

In the Organize and Cleanup Holes step, you will organize the surfaces that form holes in the model.

1. In the Hole Parameters Table, D< column, type 5 in the first row and 10 in the second row.
   Note: This will organize the holes into two collectors that will include holes ranging from 0 - 5 units and 5 - 10 units collectively.

   
   
   Figure 2.

2. Click Auto Organize.
   HyperMesh organizes all of the holes in the model less than 10 units into two component collectors, each with a different color.
3. From the Model Browser, expand the Components folder.
   Note: Two new component collectors, with the name solidholes followed by the numerical average of the diameter range of the holes, are created.

   
   
   Figure 3.

4. In the Hole Parameters Table, Num circumference Elems column, type 12 in each row.
   Note: The Num Circumference Elems field governs the number of elements that will be meshed around the hole.
5. In the Longitudinal Elem Size column, type 1 in each row.
   Note: The Longitudinal Elem Size field dictates the unit size of the elements through the length of the hole.
6. Click Auto Organize.
7. Click Accept.

In this step you will mesh holes.

1. In the Hole Parameters Table, Mesh Type column, select R-tria regular in each row.
2. Click Mesh All.
   HyperMesh creates a perfectly straight tria mesh down the length of the holes with no twisting.
3. Click ACCEPT.

In this step you will organize and clean up features.

1. In the panel area, click .
2. In the Define New dialog, type Faces in the text field.
3. Click OK.
4. Select all five of the flat faces around the circumference of the part as indicated in the following image.

   
   
   Figure 4.

5. Click proceed.
   The Organize panel opens with the surfaces pre-selected and ready to move into a new component called grp_Faces.
6. Click move.
7. Click return.
8. Click .
9. In the Define New dialog, type TopHole in the text field.
10. Click OK.
11. Rotate the model so you are looking at it from underneath into the center.
12. Select the five surfaces that are shaded gray as indicated in the following image.
    Note: You only need to select one of the two surfaces that make up a cylinder; when you click proceed HyperMesh automatically selects the other surfaces.

    
    
    Figure 5.

13. Click proceed.
14. In the Organize panel, click move.
15. Click return.
    Note: Your model should look similar to the following image, with the faces in one collector and the top hole in another. Your colors may vary slightly.

    
    
    Figure 6.

16. Click ACCEPT.

In this step you will organize and clean up fillets.

1. Click Components.
2. Select the part in an area that has not been organized into a new component so that the large purple part is selected.
3. Click proceed.
4. Verify that the Min Radius is 0 and the Max Radius is 5.
5. Select the Suppress fillet tangent edges checkbox.
6. Click Cleanup.
   Note: Many of the fillets now have an edge running down the center and the original edges are suppressed.
7. Click ACCEPT.

In this step you will mesh features.

1. In the Feature Parameters Table, set the Mesh Type for Faces to trias.
2. For TopHole, set the Mesh Type to R-tria union jack.
3. For both features, type 0.5 in the Elem Size field.
4. Click Mesh All.
   Note: Notice the distinctive Union Jack mesh pattern () in the top hole area and the connectivity of the mesh to the previously meshed holes.
5. Click ACCEPT.

In this step you will organize and clean up the remaining portion of the model.

In this step you will globally mesh the remaining model.

1. In the panel area, type 1 in the Element Size field.
2. Set Mesh Type to trias.
3. Click Mesh.
4. Click ACCEPT.

In this step you will clean up elements.

1. In the panel area, click Components.
2. Click comps.
3. Select all components.
4. Click select.
5. Click proceed.
6. Leave all values at their default (Min size = 0.25, Max FeatureAngle = 60.0, and Normals Angle = 150.0).
7. Click AutoCleanup.
   A dialog appears with a message that reads, "Cleanup process performed on 32 failed elements. No failed elements remain."

   Note: This confirms that all failed edges have been fixed and there are no further errors in the model.
8. Optional: Use the Manual tab to manually check the model for free edges and t-junctions, and fix any that are found. There is also an option to display normals. Use these options to find and fix any errors.
9. Click ACCEPT.
   Note: The Tetramesh Process Manager automatically places any elements that fail the AutoCleanup procedure in the user mark. This allows for easy retrieval of problem elements. You can employ the tools from the standard HyperMesh panels to fix these remaining elements.

In this step you will tetra mesh the model.

1. Under Float trias/quads to tetra mesh, click \.
   HyperMesh selects the surface elements under the general mesh selection option.

   Note: This option defines the selected elements as “floatable”, meaning that the diagonals of the underlying tetra elements can be flipped from the generated shell elements if HyperMesh determines a better element quality will result.
2. Under Fixed trias/quads to tetra mesh, click elems.
   HyperMesh selects the elements that represent the interior of holes and bores.

   Note: The option defines the selected elements as “fixed”, meaning HyperMesh will always adhere to the shell mesh pattern when generating the tetra elements.
3. Click mesh.
4. From the Model Browser, expand the Components folder.
5. Right-click on tetmesh and select Isolate Only from the context menu.
   The tetra mesh is displayed.
6. Open the Mask panel by clicking on the Display toolbar.
7. Press Shift + left-click, and then drag a box to include roughly half of the model.
8. Click mask.
   Note: Your tetra mesh should look similar to the following image.

   
   
   Figure 7.

In this optional step you will save your work.