DOC

# Hypermesh11.0 HM-3200 Tetrameshing

By Louis Dixon,2014-06-25 21:30
24 views 0
Hypermesh11.0 HM-3200 Tetrameshing

HM-3200: Tetrameshing

In this tutorial, you will learn about:

Volume tetra mesher

Standard tetra mesher

Checking tetra element quality

Remeshing tetra elements

HyperMesh provides two methods of generating a tetrahedral element mesh. The volume tetra mesher works directly with surface or solid geometry to automatically generate a tetrahedral mesh without further interaction from the user. Even with complex geometry, this method can often generate a high quality tetra mesh quickly and easily.

The standard tetra mesher requires a surface mesh of tria or quad elements as input, then provides you with a number of options to control the resulting tetrahedral mesh. This offers a great deal of control over the tetrahedral mesh, and provides the means to generate a tetrahedral mesh for even the most complex models.

The Tetramesh panel allows you to fill an enclosed volume with first or second order tetrahedral elements. A region is considered enclosed if it is entirely bounded by a shell mesh (tria or quad elements) where each element has material on one side and open space on the other.

Exercise

Step 1: Retrieve and view the model file.

The model for this exercise is housing.hm. Take a few moments to observe the model using

the different visual options available in HyperMesh (rotation, zooming, etc.). Only the geometry in the component cover is currently displayed. The file contains two parts

defined by a volume of surfaces. The geometry has been cleaned such that surface connectivity is proper and surface edges that would cause sliver elements are suppressed. Step 2: Use the volume tetra mesher and equilateral triangles to create a tetra mesh for the cover.

Access the Tetramesh panel from the menu bar by selecting Mesh > Create > Tetra

1. Mesh

2. Go to the Volume tetra subpanel.

3. Set the entity selector to surfs and select one of the surfaces in the model.

The connected surfaces are selected automatically.

4. Verify that 2D type: is set to trias and 3D type: is set to tetras.

These control the type of element that will be created for the surface mesh and solid mesh

of the part.

5. Select Elems to Current Comp to place the newly created elements in the current

component collector.

6. Verify that the Use curvature and Use proximity options are not active.

For element size= specify 10. 7.

8. Click mesh to create the tetra mesh.

From the toolbar, click Shaded Elements and Mesh Lines (). 9.

10. Take a moment to inspect the mesh pattern that the volume tetra mesher created.

Tetra mesh from the volume tetra subpanel and equilateral triangles (2D: trias)

11. Click reject to reject the mesh.

The mesh is deleted.

Step 3: Use the volume tetra mesher and right triangles to create a tetra

mesh for the cover.

You should still be in the Tetramesh / Volume tetra subpanel.

1. Select one of the surfaces in the model.

2. Switch 2D type: to R-trias.

3. Click mesh to create the tetra mesh.

4. Inspect the mesh pattern that the volume tetra mesher created.

Compare it to the first mesh you created and note the differences. The 2D type: R-trias

setting tends to create tetra elements with triangular faces that are right triangles

(90-45-45 angles) while the 2D type: trias setting tends to create equilateral triangles 5. (60-60-60 angles).

Tetra mesh from the volume tetra subpanel and right triangles (2D type: R-trias)

6. Click reject to reject the mesh.

Step 4: Use the volume tetra mesher to create a tetra mesh with more elements along curved surfaces.

You should still be in the Volume tetra subpanel.

1. Select one of the surfaces in the model.

2. Activate the option, use curvature.

Additional parameters appear. The option, Use curvature, causes more elements to be

created along areas of high surface curvature. Thus, curved areas such as fillets will have more and smaller elements, which capture those features with higher resolution.

For Min element size = specify 1.0. 3.

Verify that Feature angle = is set to 30. 4.

5. Click mesh to create the tetra mesh.

7. Inspect the mesh pattern that the volume tetra mesher created.

Compare it to the previous meshes you created and note the differences. More elements 8. are created around the fillets.

Tetra mesh from the volume tetra sub-panel and the option use curvature active

9. Click reject to reject the mesh.

Step 5: Use the volume tetra mesher to create a tetra mesh with more elements around small features.

You should still be in the Volume tetra subpanel.

1. Select one of the surfaces in the model.

2. Activate the Use proximity option.

The Use proximity option causes the mesh to be refined in areas where surfaces are smaller. The result is a nice transition from small elements on small surfaces to larger elements on larger, adjacent surfaces.

3. Click mesh to create the tetra mesh.

Inspect the mesh pattern that the volume tetra mesher created. Compare it to the previous

meshes you created and note the differences. More elements were created around 5. surfaces with small angles as indicated in the following image.

Tetra mesh from the volume tetra subpanel with options Use curvature and Use proximity

Step 6: Prepare the display to tetra mesh the hub component using the standard tetra mesher.

Use the HyperMesh Model Browser to turn off the display of geometry for all 1. components.

2. Turn on the display of the geometry for the hub component.

3. Use the HyperMesh Model Browser to turn off the display of elements for all components.

4. Turn on the display for the hub and tetras components for elements.

There are tria shell elements in the hub component. Currently, there are no elements in the tetras component.

Step 7 (Optional): Review the connectivity and quality of the tria mesh

to validate its integrity for the standard tetra mesher.

Use the Edges and Check Elems panels to make sure that there are no free edges or very small angles in the tria shell mesh.

Access the Edges panel from the menu bar by selecting Mesh > Check > Components >

1. Edges.

2. With the comps selector active, pick any tria element on the hub component.

3. Click find edges.

A message in the status bar should state, "No edges found. Selected elements may enclose a volume."

This is desired as the tetra mesher requires a closed volume of shell elements. 4. Click return to exit to the main menu.

Access the Check Elements panel from the menu bar by selecting Mesh > Check >

5. Elements > Check Elements.

6. Verify that you are in the 2-d subpanel.

7. Identify elements having an aspect ratio greater than 5.

Aspect ratio is the ratio of the longest edge of an element to its shortest edge. This check

helps you to identify sliver elements.

All of the hub’s shell elements pass the check; all of the elements have an aspect ratio less than 5.

8. Identify tria elements having an angle less than 20. (trias: min angle)

This check also helps you to identify sliver elements. All the hub’s shell elements pass the check; all the elements have angles greater than 20.

The surface mesh is suitable for creating a tetra mesh. 9. Click return to exit to the main menu.

Step 8: Create a tetra mesh for the hub using the standard tetra mesher.

1. Use the HyperMesh Model Browser to set the current component to tetras.

Access the Tetramesh panel from the menu bar by selecting Mesh > Create > Tetra

2. Mesh.

3. Enter the Tetra mesh subpanel.

With the comps selector active under Float trias/quads to tetra mesh, select one of the

4. hub shell elements from the graphics area.

Using this option, HyperMesh will swap the diagonal for any pair of surface trias that will

result in a better tetra mesh quality. If you would rather keep the diagonal, see sub-step 5

(Optional) To keep the diagonal as is, select the comps selector under Fixed trias/quads

5. to tetra mesh.

6. Click mesh to generate the tetrahedral elements.

Cut-away view of tetrahedral elements

Step 9: Check the quality of the hub’s tetra elements.

Use the HyperMesh Model Browser to display only the elements in the tetras

1. component.

2. Access the Check Elements panel.

3. Go to the 3-d subpanel.

4. Identify the smallest element length among the displayed elements.

If the minimum length is acceptable for a target element size of 5.0, then no further action is necessary.

5. Identify the smallest angle (tria faces: min angle) among the displayed elements.

If the minimum tria face angle is no less than 10?, then the mesh quality should be acceptable.

6. Identify elements having a tet collapse smaller than 0.2.

The tet collapse criteria is a normalized volume check for tetrahedral elements. A value of 1 indicates a perfectly formed element with maximum possible volume. A value of 0 indicates a completely collapsed element with no volume.

The message bar indicates that one element has a tetra collapse smaller than 0.2. Step 10: Isolate the element with the tetra collapse smaller than 0.2 and find the elements surrounding it.

You should still be in the Check Elements panel.

With 0.2 still specified for tet collapse, click tet collapse again. 1.

2. Click save failed.

The element that failed the tetra collapse check is saved in the user mark, and can be retrieved in any panel using the extended selection menu.

Access the Mask panel from the Display toolbar by selecting Mask (). 4.

You can also press F5 on your keyboard to enter the Mask panel.

5. Set the entity selector to elems and select elems >> retrieve.

The element that was saved in the Check Elements panel is retrieved.

6. Select elems >> reverse.

Only the one tetra element that failed the tetra collapse check should be displayed. 8. Click return to exit to the main menu.

The layer of elements that is attached to the one displayed element is identified and displayed.

The layer of elements that is attached to the displayed elements is identified and displayed. The functionality of unmask adjacent can be duplicated using the Find panel, find

attached subpanel on the Tool page.

Step 11: Remesh the hub’s displayed tetra elements to improve their tetra collapse.

1. Access the Tetramesh panel.

2. Go to the Tetra remesh subpanel.

3. For 3D elements, select elems >> displayed.

4. Click remesh to regenerate this area of the mesh.

Note that the re-meshing operation works on only one group of elements (one volume) at a time.

6. Access the Check Elements panel.

7. Click tet collapse to find out if the tetra collapse has improved for the displayed elements.

The message in the status bar should indicate that the minimum tetra collapse is larger than the value reported before the tetra elements were remeshed.