HM-3210: Create a Hex-Penta Mesh Using Surfaces

In this step you will open and review the model file, arm_bracket.hm.

1. Start HyperMesh Desktop.
2. From the menu bar, click File > Open > Model.
3. In the Open Model dialog, open the arm_bracket.hm model file.

In this step you will mesh the top surface of the base, including the L-shaped surface.

1. In the Model Browser, Component folder, right-click on base and select Make Current from the context menu.
2. Right-click on base again and select Isolate from the context menu.
   HyperMesh hides all components except for base.
3. Open the AutoMesh panel by clicking Mesh > Create > 2D AutoMesh from the menu bar.
4. Go to the size and bias subpanel.
5. Shade the model's geometry and surface edges by clicking on the Visualization toolbar.
6. Verify that the entity selector is set to surfs.
7. Select the surfaces on the top of the base, including the L-shaped surface at the intersection of the base and the arm.

   
   
   Figure 2.

8. Set the meshing mode to automatic.
9. In the element size field, type 10.
10. Set the mesh type to quads only.
11. Click mesh.
    The selected surface is meshed.

    
    
    Figure 3.

12. Return to the main menu by clicking return.

In this step you will create layers of hex elements for the base.

1. Open the Elem Offset panel by clicking Mesh > Create > 3D Elements Element Offset from the menu bar.
2. Go to the solid layers subpanel.
3. Click elems to offset: elems >> displayed.
   HyperMesh selects the elements on the base.
4. In the number of layers= field, type 5.
5. In the total thickness= field, type 25.
6. Click offset+.
   The hexa mesh is created.

   
   
   Figure 4.

In this step you will prepare the display for meshing the arm's curved segment.

1. In the Model Browser, Component folder, right-click on arm_curve and select Show from the context menu.
2. Open the Mask panel by pressing F5.
3. Click elems >> by config.
4. Click config= and select the hex8 configuration.
5. Click select entities.
   HyperMesh selects the elements with a configuration of hex8 in the model.
6. Click mask.
   The element is masked.
7. Return to the main menu by clicking return.

In this step you will create a node at the center of the arm radius.

1. Open the Distance panel by pressing F4.
2. Go to the three nodes subpanel.
3. Verify that the N1 node selector is active.
4. While pressing the left mouse button, move it over the curved line as indicated in the following image, and then release it when the cursor changes to .
   HyperMesh highlights the line.

   
   
   Figure 5.

5. Click three locations along the selected line. The active selector advances from N1 to N2 to N3, and HyperMesh creates the temporary nodes on the selected curved line of the arm.
6. Click circle center.
   The node is created at the center.

   Note: You will use this node in the next step when you mesh the arm.

   
   
   Figure 6.

7. Return to the main menu by clicking return.

In this step you will create hexa elements in the curved portion of the arm using spin.

1. In the Model Browser, Component folder, right-click on arm_curve and select Make Current from the context menu.
2. Open the Spin panel by clicking Mesh > Create > 3D Elements > Spin from the menu bar.
3. Go to the spin elems subpanel.
4. Click 2d elems: elems >> by window.
5. Select the plate elements within the L-shaped cross section of the arm as indicated in the following image.

   
   
   Figure 7.

6. Click select entities.
7. In the angle= field, type 90 degrees.
8. Set the orientation vector to x-axis (Y-Z plane).
9. Select the center node you created in step 5 for the base node (B).
10. In the on spin= field, type 24.
    Note: This option determines how many layers of hex elements HyperMesh creates when the plate elements are spun.
11. Click spin-.
12. Return to the main menu by clicking return.

    
    
    Figure 8.

In this step you will create faces on hex elements.

1. Open the Faces panel by clicking Mesh > Check > Components > Faces from the menu bar.
2. Set the entity selector to comps.
3. Click comps >> arm_curve.
4. Click select.
5. Click find faces.
   HyperMesh creates 2D shell elements on the free faces of every 3D solid element in the component and places them in a new component named ^faces.

   Note: The ^faces component is created with its visualization set to wireframe, therefore you will not be able to see the new elements right away if the arm_curve component is displayed and in shaded mode.
6. Shade the model's elements and mesh line by clicking on the Visualization toolbar.
   The graphics area now displays the elements in the ^faces component.

In this step you will prepare the display for meshing the second arm segment.

In this step you will mesh the L-shaped set of surfaces between the arm_straight and boss components.

1. In the Model Browser, Component folder, right-click on arm_straight and select Make Currrent from the context menu.
2. Open the Automesh panel.
3. Select the three surfaces lying on the intersection between the arm_straight and boss components as indicated in the following image.
   Note: These surfaces are all in the arm_straight component.

   
   
   Figure 9.

4. Set the meshing mode to interactive.
5. Click mesh. The meshing module opens.
6. Go to the density subpanel.
7. Adjust the density of each edge to obtain a mesh that matches the following image.
   Note: This mesh pattern matches the mesh pattern at the intersection of the two arm segments. This is necessary for the next step.

   
   
   Figure 10.

8. Click mesh. The mesh density is updated.
9. Create the elements and go back to the main menu by clicking return twice.

In this step you will use linear solid to build the mesh between the two set of shell elements.

1. Open the Linear Solid panel by clicking Mesh > Create > 3D Elements > Linear 3D from the menu bar.
2. Activate the from: elems selector.
3. Select the ^faces elements lying on the intersection between the first and second arm segments as indicated in the following image.
   Note: Quickly select all of the necessary elements by selecting one of the elements and then clicking from: elems >> by face.

   
   
   Figure 11.

4. Activate the to: elems selector.
5. Select the shell elements between the arm and boss that you created using the Automesh panel in Step 9.
6. Activate the from: alignment: N1 selector.
7. Select three nodes on one of the "from elements" that you selected in step 10.3 as indicated in the image that follows.
8. Activate the to: alignment: N1 selector.
9. Select three nodes on the "to element" that corresponds to the "from element" with the three "from nodes" as indicated in the following image.

   
   
   Figure 12.

10. In the density= field, type 12.
11. Click solids.
    The mesh is created.

    
    
    Figure 13.

12. Return to the main menu by clicking return.

In this step you will prepare the display for meshing the boss.

In the Model Browser, Component folder, right_click on boss and select Show from the context menu.

Figure 14.

In this step you will create a shell mesh on the bottom of the boss.

1. In the Model Browser, Component folder, right-click on boss and select Make Current from the context menu.
2. Open the Automesh panel.
3. Select the five surfaces on the bottom face of the boss as indicated in the following image.

   
   
   Figure 15.

4. Click mesh.
   The meshing module opens.
5. Adjust the density of each edge to obtain a mesh that matches the following image.

   
   
   Figure 16.

6. Click mesh.
   The mesh density is updated.
7. Return to the main menu by clicking return twice.

In this step you will project a node to the bottom face of the boss.

1. Open the Project panel by clicking Mesh > Project > Nodes from the menu bar.
2. Go to the to line subpanel.
3. Select the node on the rightmost top vertex as indicated in the image that follows.
4. Click nodes >> duplicate.
5. Activate the to line: line list selector.
6. Select the line on the boss's top face as indicated in the following image.

   
   
   Figure 17.

7. Set the along vector to x-axis.
8. Click project.
   The node projects to the line.
9. Return to the main menu by clicking return.

In this step you will generate hexas for the boss using the Solid Map panel.

1. Open the Solid Map panel by clicking Mesh > Create > Solid Map Mesh from the menu bar.
2. Go to the general subpanel.
3. Click the source geom switch and select none.
4. Activate the dest geom: surf selector.
5. Select the top surface of the boss as indicated in the following image.

   
   
   Figure 18.

6. Click the along geom switch and select mixed.
7. Activate the along geom: mixed lines selector.
8. Select the line indicated in the image that follows.
9. Activate the along geom: mixed node path selector.
10. Select the 13 nodes as indicated in the following image, to define the exact location of the solid element layers.
    Note: A total of 13 nodes should be selected, starting at the boss mesh, and then using all of the nodes along the edge of the arm_straight component, ending with the node projected to the top of the boss.

    
    
    Figure 19.

11. Click elems to drag: elems >> by collector >> boss.
12. Click select.
13. Click mesh.
    HyperMesh creates the elements and completes the mesh on this part.

    
    
    Figure 20.

14. Return to the main menu by clicking return.

In this optional step you will check the connectivity of the model.

1. Go to the Faces panel.
2. Click comps.
   A list of components displays.
3. Select every component from the list, or select comps >> all.
4. Click select.
5. Click find faces.
6. From the Model Browser, turn off the geometry display of all components.
7. Turn off the element display of all components except ^faces.
8. Exit the panel by clicking return.
9. From the Post page, select hidden line.
10. Select the xz plane and trim plane checkboxes.
11. Click show plot.
    HyperMesh displays the faces with a plane cutting the model in half.

    Note: This allows you to review the interior of the model.
12. Click near the cutting plane, hold the left mouse button down, and move your mouse back and forth.
    The cutting plane moves through the model, allowing you to see if any face elements exist on the interior of the model.

    Note: You should see that there are face elements interior to the model, between the boss and arm. You need to perform some corrections on the connectivity.

    
    
    Figure 21.

13. Return to the main menu by clicking return.

In this optional step you will correct the connectivity of the model.

1. In the Model Browser, display the elements for all components except ^faces.
2. Display the model's elements as transparent by clicking on the Visualization toolbar.
3. Go to the Faces panel.
4. Set the entity selector to elems.
5. Click elems >> displayed.
6. Click preview equiv.
   HyperMesh highlights coincident nodes on the intersection between the arm and the boss.
7. Specify a slightly larger value in the tolerance= field and then click preview equiv.
   HyperMesh identifies more coincident nodes on the intersection.
8. Repeat Step 16.7 until all 60 coincident nodes have been found.
9. Click equivalence.
   HyperMesh replaces the nodes to the location of the lowest node ID.
10. Switch all the components to the shaded visual mode.

In this optional step you will recheck the connectivity of the model.

In this optional step you will save your work.