Exercise: Creating a Solid Mesh

Exercise: Creating a Solid Mesh
This exercise uses the model file, model_gear.hm. This exercise illustrates how to
create a solid mesh by first splitting the solid into mappable regions and then use the
Solid Map panel.
Step 1: Retrieve and review model file.
1. Open the model_gear.hm file.
!
The model consists of a surface geometry of a gear. Because the surfaces enclose a
volume, a solid can be created Notice that the model can be simplified by only working
with 1/6th of the model. The solid needs to be split into mappable regions and a shell
mesh can also be created as a guide for the solid mesh.
Step 2: Create a solid from surfaces that enclose a volume
1. Using the main menu, select Geometry > Create > Solids > Bounding Surfaces.
Because the surfaces enclose a single volume, a solid can be created.
2. Activate Auto select solid surfaces.
This allows us to select only one surface and HyperMesh will select the remaining
surfaces that enclose the volume.
3. Click on surfs and then select one of the surfaces in the graphics area.
4. Select create.
Once create is selected, a solid is created.
Notice that the solid is colored green, as that is the 3D Topology color for a solid.
Step 3: Split the solid into a repeatable region
1. Temporary nodes need to be created to help define the planes where the splitting will
occur. To create these nodes, select Geometry > Create > Nodes > Arc Center.
This allows us to create temporary nodes at center of the lines in the model.
2. Click on lines and then select the line indicated in the image below.
3. Select create. Notice that a node is created at the circle center of the selected line.
4. Repeat substeps 1-3 to create a node at the circle center of the two lines indicated in
the image below.
This results in the following nodes being created:
5. Next the node in the center of the smaller circle needs to be duplicated and rotate +
and – 30 degrees to allow us to define two planes and cut a 1/6 portion of the model.
Select Geometry > Rotate > Nodes from the main menu to enter the Rotate panel.
6. Select the node in the center of the small hole in the graphics area and then in the
Rotate panel select nodes >> duplicate.
7
Select the x-axis as the axis to rotate about and then click on B and select one of
the nodes in the center of the model.
8. Set the angle to 30 and then click on rotate + to rotate the node 30 degrees.
9. Repeat substeps 6-8, this time selecting rotate – to rotate the node 30 degrees in
the opposite direction.
10. Select Geometry > Edit > Solids > Trim with Plane/Surfaces to enter the Solid
Edit panel.
11. In the with plane column, click on solid and then select the solid in the graphics
area.
12. Click on N1 in the panel and then select N1 N2 N3 and B as shown in the image
below (notice that N3 and B are the same node):
13. Click on trim to trim the solid.
14. Repeat substeps 11-12, this time selecting N1 as the node that was rotated -30
degrees. This results in 3 solids.
15. From Tools page, enter the Delete panel and delete the 2 extra solids. You should
be left with the following in the graphics area:
Step 4: Trim the solid using the Solid Map panel, trim with ilnes subpanel
1. From the menu bar, select Geometry > Edit > Solids > Trim with Lines.
2. Using the with bounding lines option, click on solids and then select the solid in
the graphics area.
3. Click on lines and then select two of the parallel lines defining one of the ribs
(as shown below).
4. Click on trim to trim the solid.
5. Repeat substeps 2-4 twice using the other two sets of parallel lines to completely
trim the rib.
6. Repeat substeps 2-5 to trim the other rib.
7. The next place to be trimmed is along the curvature using the trim with sweep lines
option. Under with sweep lines column, click on solids and then select the large
solid in the graphics area.
8. Click on lines and then select the highlighted lines below (there are 7 lines).
9. Under sweep to select by vector and then select N1 and N2 as indicated in the
image below:
9. Select trim to trim the solid.
Step 5: Simplify the 2D Topology to make the solid mappable.
1. Enter the Mask panel by selecting the Tool page and selecting mask.
2. Set the entity selector to solids and select all solids except the curved solid we just
trimmed. Select mask. This leaves you with the following solid displayed:
One rule for mappable solids is that the vertices have to be clearly defined from the
source to the destination surface. This is the first issue that we will fix.
3. Enter the Quick Edit panel by selecting Geometry> Quick Edit.
4. Next to project point, click on point(s) and then select the point highlighted in the
image below:
5. Next to point(s) click on lines and then select the circular line indicated above.
6. Next use those 2 points to split the surface. Next to split surf-node click on node
and then select one of the two points highlighted below. The selection will
automatically move to the second node. Select the other point in the image below to
trim the surface.
7. Using this new point, the side of the cylinder is split using the split surf-line option.
Click on node and select the point indicated in the image below. Then click on line
and select the line indicated to trim the side of the cylinder.
8. Repeat substeps 4-7 on the opposite side to result in the following topology:
9. Another area where the vertices need to be defined better is shown in the following
image. Again, the split surf-node option is used. Select the two nodes indicated in
the image below.
10. Repeat substep 9 on the opposite side. This results in the following topology.
!
11. The last step is to equivalence the shared edges so that there is a single destination
face. Within the Quick Edit panel, click on line(s) next to toggle edge and then
select the edges shown in the image below (there are 10 lines):
This results in the following topology:
!
12. Unmask all the solids and change the geometry view to Mappable to see which
solids are currently considered mappable.
Currently only the solid we just edited is considered mappable.
Step 6: Use the Solid Edit, trim with planes/surf subpanel to make the final
trims to the solid
1. To enter the Solid Edit panel, select Geometry > Edit > Solids > Trim with
Plane/Surfaces.
2. Using the with plane option, click on solids and then select the large solid in the
graphics area.
3. Click on N1 and then define N1 N2 N3 and B on the surface on the side of the rib, as
shown below:
4. Click trim to trim the solid.
5. Repeat substeps 2-4 three more times to make 4 trims along the planes defined by
the ribs.
6. One final area to trim using the with plane option is at the very top of the gear where
the ribs end. First, select the 5 solids shown in grey in the image below:
7. Click on N1 and define N1 N2 and N3 on the top of the middle solid and B at the top
of the left rib, as shown in the image above.
8. Select trim to trim the solids.
Step 7: Finish geometry cleanup to make all solids mappable
1. Change the view to Mappable. Notice how only 1 solid is now not mappable.
Closely inspecting the topology, we find that there is one line that is currently shared
that is making the solid unmappable.
2. Rotate and zoom into the area shown below.
3. Return to the Quick Edit panel by selecting Geometry > Quick Edit.
4. Use the toggle edge option to suppress the edge indicated in the image above.
By toggling this surface and making it suppressed, the solid is now mappable and
now all solids are mappable.
Step 8: Create 2D mesh on surfaces and associate nodes to surfaces when
necessary
1. Enter the Automesh panel by selecting Mesh > Create > 2D Auto Mesh from the
menu bar.
2. Rotate and the model to select the surfaces shown below:
3. Set the element size to 1.5 and the mesh type to quads.
4. Click mesh.
5. Change the element density so that the top surface is 2 elements by 5 elements and
the bottom surface is 3 elements by 7 elements.
6. Click mesh and then return to accept the mesh.
7. Next the curved surfaces shown below are meshed with the same element size and
type, and the edge densities are 5 elements by 10 elements on all surfaces (the
middle one has bottom edges of 2, 6, 2):
8. Next the round feature will be shell meshed. The larger surface defining the feature
is meshed first. Below shows the edge densities used:
9. To fill the smaller surface representing the circular feature, the Ruled panel is used.
To enter the Ruled panel, select Mesh > Create > 2D Elements > Ruled.
10. Set the first selector to line list and select the line indicated in the image below.
Then set the second selector to node list and select the nodes in the image below:
11. Set the selection to mesh, w/o surf and click create. Then select return to exit the
panel.
12. Next the Edges panel is used to equivalence duplicate nodes. From the Tool page
select edges.
13. Click on comps and select the lvl1 component.
14. Set the tolerance value to 0.1 and then click preview equiv.
15. Select equivalence and then click return to exit the panel.
16. The newly created nodes now need to be associated to the surface. This is done by
selecting Geometry > Edit > Nodes > Associate to enter the Node Edit panel.
17. Set the geometry selector to surfs and select the underlying surface.
18. Click on nodes, select one of the nodes from the newly created elements and then
select nodes >> by face.
19. Set the tolerance value to 0.2 and click associate.
20.The last step is to create a shell mesh on the surface shown below. Return to the
Automesh panel by selecting Mesh > Create > 2D Auto Mesh from the menu bar.
21. Select the surface shown above and set the element size to 1.5 and then mesh
type to quad.
22. Click mesh and then select return to accept the mesh.
Step 9: Use the Solid Map panel to create the hexa mesh.
1. The Solid Map panel will be used to create the hexa mesh. Access this panel by
selecting Mesh > Create > Solid Map Mesh.
2. Select the multi solids subpanel.
3. Select solids >> displayed to select all the solids in the model.
4. Set the elem size to 1.5 and then source shells to quads.
5. Verify that interactive, elems to solid/surf comp and show solid id are selected,
and then click mesh.
Two things occur here. First, where shells don’t exist for extrusion, HyperMesh
creates them and produces a preview mesh that can be edited, just like the
Automesh panel. Second, the order and direction in which the solids will be meshed
is displayed; the order is indicated by a number and the direction is represented by a
line.
6. Select mesh again to create the solid elements and then click return.
Step 10: Complete the mesh by duplicating and rotating the solid elements
to completely represent the part.
1. First we need to delete the shell elements as they are no longer necessary. From
the menu bar select Mesh > Delete > Elements.
2. Select elems >> by config and then set config= to quad4.
3. Click select entities and then select delete entity.
4. Repeat substeps 2-3 to delete the tria3 elements.
5. In order to duplicate and rotating the solid elements, the Rotate panel is used. Enter
the Rotate panel by selecting Mesh > Rotate > Elements.
6. Select the YZ Front Plane View,
.
7. Select elems >> displayed and then select elems >> duplicate to duplicate the
displayed elements. From the pop-up that appears select original comp.
8. Set the axis for rotation to x-axis and the base point (B) as one of the nodes in the
center of the model (if you no longer have this temporary node, simply use the Node
panel, Arc Center subpanel to create it again).
9. Set angle = to 60 and then click rotate +.
10. The elements that were just rotated are still selected. Simply select elems >>
duplicate, original comp again and then click rotate +.
11. Repeat substep 10 until the model is fully represented with solid elements.
12. From the Tool page, select edges to enter the Edges panel.
13. Select the lvl1 component and then select preview equiv.
14 Select equivalence to merge the duplicate nodes and complete the solid mesh.