HM-2035: Refine Topology

In this step you will open the model file, clip_refine.hm.

1. From the menu bar, click File > Open > Model.
2. In the Open Model dialog, open the clip_refine.hm model file.
3. Take a few moments to observe the model using the different visual options available in HyperMesh (rotation, zoom, etc.).

In this step you will create a preliminary mesh.

1. To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.
2. Set the entity selector to surfs.
3. Go to the size and bias subpanel.
4. In the element size = field, type 2.5.
5. From the mesh type list, select mixed.
6. Switch the meshing mode from interactive to automatic.
7. Click surfs >> displayed.
8. Click mesh.
   HyperMesh meshes the surfaces.

   
   
   Figure 1.

In this step you will review the mesh quality.

1. Take a minute to rotate, zoom, and pan the model to review the mesh that was created. Pay attention to the locations where the mesh was not created in rows and columns of quads.
2. To open the Check Elements panel, click Mesh > Check > Elements > Check Elements from the menu bar, or press F10.
3. Go to the 2-d subpanel.
4. In the length < field, type 1.
5. To evaluate the minimum length, click length.
   HyperMesh highlights the elements that failed the check.
6. To exit the panel, click return.
7. In the Model Browser, Component folder, click next to Middle Surface to turn off the display of its elements.

In this step you will remove short edges by combining fixed points.

1. To open the Replace panel, click Geometry > Edit > Fixed Points > Replace from the menu bar.
2. Verify that the moved points selector is active.
3. Select the lower fixed point as indicated in the image below.
   Note: If there are no visible fixed points on your model, verify that is selected on the Display toolbar.
4. Activate the retained point selector.
5. Select the upper fixed point as indicated in the image below.
6. Click replace.

   
   
   Figure 2.

In this step you will remove the fixed points interior to all surfaces.

1. Go to the suppress subpanel.
2. Under at cursor, verify that the point selector is active.
3. Select the four fixed points as illustrated in the following image.
   HyperMesh deletes each fixed point when you select it.

   
   
   Figure 3.

   These fixed points are left over from a defeaturing operation where small holes (pinholes) were removed. They could remain without greatly sacrificing the element quality, given the element size used for the mesh, but the mesh would be better without them.

4. To exit the panel, click return.

In this step you will add edges to the surfaces to control the mesh pattern.

1. To open the Trim with Nodes panel, click Geometry > Edit > Surfaces > Trim with Nodes from the menu bar.
2. Under node normal to edge, click node.
3. Zoom into the area illustrated in the image below and select the indicated fixed point.
4. With the lines selector now active, select the line shown in the image below.
   HyperMesh creates an edge from the location of the fixed point perpendicular to the line.

   
   
   Figure 4.

5. Repeat Steps 2 through 4 for the point and line illustrated in the following image.

   
   
   Figure 5.

6. Repeat Steps 2 through 4 for the point and line illustrated in the following image.

   
   
   Figure 6.

7. Repeat Steps 2 through 4 for the point and line illustrated in the following image.

   
   
   Figure 7.

In this step you will continue to add edges to surfaces to control the mesh pattern.

1. Go to the trim with surfs/planes subpanel.
2. In the with plane column, verify that the surfs selector is active.
3. Select the five surfaces indicated in the following image.

   
   
   Figure 8.

4. Verify that the direction selector is set to N1, N2, N3.
5. Click N1 to make the selector active.
6. Press and hold the left mouse button, move it over the edge as indicated in the following figure, and then release it when the cursor changes to a square with a dot in the center .
7. Click two points anywhere along the edge. Do not click a third.
   HyperMesh places nodes on the line for N1 and N2.
8. To open the Distance panel, press F4.
9. Go to the three nodes subpanel.
10. Press and hold the left mouse button, move it over the edge of the hole as indicated in the following image, and then release it when the cursor changes to a square with a dot in the center .

    
    
    Figure 9.

11. Click three points anywhere along the edge.
    HyperMesh places temporary nodes on the line representing N1, N2, and N3.

    Note: The technique you used to create nodes to select where none existed before can be used in any place where nodes need to be selected but do not exist in the model. You can create nodes in this manner on lines, surfaces and elements. For more details, see the HyperMesh online help. Pick the index and type, Picking Nodes on Geometry or Elements.
12. Click circle center.
    HyperMesh creates a node at the center of the hold.
13. To exit the Surface Edit panel, click return.
14. Activate the B selector.
15. Select the node that was just created at the center of the hole.
16. Click trim.
    HyperMesh trims the surfaces through the center of the hole.
17. To exit the panel, click return.

In this step you will suppress shared edges causing a small edge.

1. To go to the (Un)suppress panel, click Geometry > Edit > Surface Edges > (Un)Suppress from the menu bar.
2. Select the five lines illustrated in the following image.

   
   
   Figure 10.

3. Click suppress.
   HyperMesh suppresses each line, which is indicated by a blue, dashed line.

In this step you will remesh the surfaces of the part using the automatic mode, a size of 2.5, and the mixed mesh type.

1. In the Model Browser, Component folder, click next to Middle Surface to display its elements.
2. To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.
3. Verify that elem size = is set to 2.5 and the mesh type is set to mixed.
4. To select all displayed surfaces, click surfs >> displayed.
5. Click mesh.

In this step you will again review the mesh quality.

1. Take a minute to rotate, zoom, and pan the model to review the mesh that was created. The mesh consists completely of rows and columns of quads.
2. To open the Check Elements panel, click Mesh > Check > Elements > Check Elements from the menu bar, or press F10.
3. Go to the 2-d subpanel.
4. In the length < field, type 1.
5. To evaluate the minimum length, click length.
   HyperMesh highlights only two elements that failed the check. Both of these elements failed the check because of the shape of the part. These elements are not too small compared to the global element size, therefore you can leave them as is.
6. To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.
7. Go to the QI optimize subpanel.
8. Verify that elem size = is set to 2.5 and the mesh type is set to mixed.
9. Click edit criteria.
10. In the Criteria File Editor dialog, type 2.500 in the Target element size field.
11. Click Apply.
12. Click OK.
13. To select all displayed surfaces, select surfs >> displayed.
14. Click mesh.
    HyperMesh replaces the old mesh with a new mesh.
15. If there is a message saying, "There is a conflict between the user requested element size and quality criteria ideal element size," click the Recompute quality criteria button using a size of 2.5.
16. To access the Quality Index panel, click Mesh > Check > Elements > Quality Index from the menu bar.
17. Go to page 1.
18. Verify that the comp.QI is 0.01. This low value indicates that the mesh is good quality. The higher the number, the lower the mesh quality.

In this step you will save your work.