17.11.9 An example including bottom-up meshing techniques

The following is a step-by-step example of meshing a part using a combination of top-down and bottom-up methods. The procedures and images describe one way that you can create a hexahedral mesh for this part. Before you begin, you should be familiar with top-down meshing, creating partitions, and using the Edit Mesh toolset. You should also have read the sections discussing bottom-up meshing, mesh-geometry associativity, and related techniques:

The example part (bottomup_mesh_example_part.sat) is imported from an ACIS file. The file is included with the Abaqus installation, and you can use the following utility to obtain a copy:

abaqus fetch job=bottomup_mesh_example_part.sat

For more information about ACIS files, see “Importing parts from an ACIS-format file,” Section 10.7.4.

Figure 17–104 shows the original part. There are three solid regions; the regions colored green and yellow can be meshed using the top-down structured and swept meshing techniques, respectively, and the orange region is unmeshable with the automated top-down techniques and hexahedral elements.

Figure 17–104 Default mesh color coding on the imported part.

Partitioning the unmeshable region and meshing the top-down regions

To mesh the part, we will first create three partitions. The first two partitions create another top-down swept meshable region near the outer edge of the unmeshable region. The third partition is a face partition that you will use later as a vector for the bottom-up extrude method. You could apply bottom-up meshing techniques to the entire unmeshable region without partitioning. However, the resulting mesh would contain some poorly formed elements near the outer edge. In practice, you may create several bottom-up meshes before you make a satisfactory mesh for the entire region. Especially for more complex parts, you may want to save copies of a part with different meshing approaches until you decide which approach yields the best mesh.

Partitioning the unmeshable region:

Rotate the part so that you are viewing the bottom of the part, as shown in Figure 17–105.
Figure 17–105 Creating an offset partition on the bottom face.
Complete the following steps to partition the face:
1. From the partition face tools in the module toolbox, select the sketch method tool .
2. Select the bottom face of the part, and select one of the straight edges to be vertical and on the right.
  Abaqus/CAE opens the Sketcher.
3. From the Sketcher toolbox, select the offset tool .
4. Select the curved edge, and click mouse button 2 to accept the selected edge.
5. Enter 2.5 in the prompt area as the offset distance.
  Abaqus/CAE displays a preview of the offset partition.
6. Click OK if the offset is shown correctly (toward the interior of the part), or click Flip if the offset is shown outside the part.
7. Click mouse button 2 or click Done in the prompt area to partition the face.
Abaqus/CAE returns to the Mesh module and displays the partitioned face as shown in Figure 17–105.
Extrude the face partition through the region.
1. From the partition cell tools in the module toolbox, select the extrude/sweep method tool .
2. Select the face partition created in Step 1 as the edge to extrude.
3. Click Extrude Along Direction in the prompt area, and pick the edge shown in Figure 17–106.
  Figure 17–106 Extruding the face partition through the cell.
4. Click OK if the extrusion direction is shown correctly (through the region), or click Flip to change the direction.
5. Click Create Partition to partition the cell.
  Abaqus/CAE displays the outer region of the part in yellow, indicating that it can now be meshed using top-down swept meshing.
Partition the front face of the unmeshable region as shown in Figure 17–107.
Figure 17–107 Creating face partitions.
1. From the partition face tools in the module toolbox, select the sketch method tool .
2. Select the front face of the unmeshable region, and select an edge to be vertical and on the right.
  Abaqus/CAE opens the Sketcher.
3. Use the vertical construction line tool to create a construction line as shown in Figure 17–108.
  Figure 17–108 Using a vertical construction line to partition the face.
4. Use the connected lines tool to create a line connecting the two points where the vertical construction line intersects the face of the part.
5. Create a second line connecting the upper point of the vertical line to the point where the fillet ends on the front face—the line should be nearly horizontal.
6. Click mouse button 2 or click Done in the prompt area to partition the face.
There are now three regions in the part that you can mesh using the top-down meshing techniques.
Assign global edge seeds to the entire part using an approximate size of 0.9 and the default settings for curvature control.
Select MeshPart from the main menu bar to mesh the top-down regions.
Abaqus/CAE highlights the unmeshable region and displays a warning that you cannot mesh it automatically.
Click OK to mesh the three top-down regions. Figure 17–109 shows the resulting partial mesh.

Figure 17–109 Automatic meshing of the top-down regions.

Beginning the bottom-up mesh

Now that the top-down mesh is complete, you can assign the bottom-up meshing technique and begin creating a hexahedral mesh for the rest of the part.

Creating a bottom-up swept mesh:

Use the mesh controls tool to assign the bottom-up meshing technique to the unmeshable region.
Abaqus/CAE colors the region light tan.
Select MeshCreate Bottom-Up Mesh from the main menu bar.
Tip: You can also click the tool in the Mesh module toolbox. (For more information, see “Using the Mesh module toolbox,” Section 17.15.)
Abaqus/CAE displays the Create Bottom-Up Mesh dialog box and makes the unmeshed regions translucent. The degree of translucency is determined by the translucency slider, located in the Color Code toolbar (for more information, see “Changing the translucency,” Section 77.3). In a more complex part, translucency allows you to select internal regions more easily.
Select the Sweep method, and click Select to the right of Source side.
Select the semi-circular face at the bottom of the protrusion, colored magenta in Figure 17–110, as the source side of the first bottom-up mesh; and click Done in the prompt area.
You must change the default selection options to select the interior face (for more information, see “Using the selection options,” Section 6.3).
Figure 17–110 Selecting a geometric face as the source side.
Tip: You can also choose two-dimensional elements or element faces as sides of a bottom-up mesh. In this case an alternative source side selection would be all the element faces on the bottom of the swept mesh.
Toggle on Connecting sides, and click Select. Rotate the part as needed to select the three faces that represent the fillet between the top protrusion and the body of the part and the corresponding flat face on the front of the part, colored yellow in Figure 17–111.
Figure 17–111 Selecting the connecting sides.
Click Done in the prompt area to end selection.
Click Mesh in the Create Bottom-Up Mesh dialog box to create the mesh.
Figure 17–112 Bottom-up swept mesh of the filleted area.
The mesh extends approximately as far into the region as the selected connecting sides, the bottom-up region remains selected, and the Create Bottom-Up Mesh dialog box remains open for the next step.

Continuing the bottom-up mesh

There are at least three methods that you can use to complete the mesh for the part. The simplest method would be to create another swept mesh, using the bottom of the mesh that you just completed and the two faces extending out from the fillet on the top of the remaining unmeshed area as the source side, the three geometric vertical faces and the set of vertical element faces as the connecting sides, and the unmeshed portion of the bottom face as the target side. This method would complete the part mesh in a single bottom-up meshing step, and the elements would be fully associated with the selected faces. You could also use the bottom-up extrude method with the bottom face of the part as the extrude distance. However, for demonstration purposes we will use a longer process that combines use of the bottom-up extrude method, the associativity tool, and the Edit Mesh toolset.

Creating a bottom-up extruded mesh:

Select the Extrude method, and click Select to the right of Source side.
Select the element faces at the bottom of the previous bottom-up mesh, as shown in Figure 17–113, as the source side for the second bottom-up mesh.
Figure 17–113 Selecting element faces as the source side.
Click Done in the prompt area to accept the selected faces.
The Create Bottom-Up Mesh dialog box reappears.
Click the Select button to choose a vector for the extruded mesh.
Select the upper endpoint of the partition as the starting point of the vector, and select the lower endpoint as the end of the vector. Figure 17–114 shows the extrusion vector.
Figure 17–114 Selecting the vector for the bottom-up extruded mesh.
Enter 10 for the Number of layers.
There are 10 elements on the inner face of the top-down swept mesh. Using the same number of elements for the extruded mesh will provide a better match when you create the third, and final, bottom-up mesh.
Verify that the extrude depth is set using the default Use vector length method, and click Mesh in the Create Bottom-Up Mesh dialog box to create the mesh.
Figure 17–115 The bottom-up extruded mesh.

The extruded bottom-up mesh ends near the bottom face of the region, as dictated by the nonplanar source side and the length of the extrusion vector. You can edit the nodes in the last extruded element layer so that they end exactly on the bottom face of the region.

Extending the extruded mesh:

Select the Edit Mesh toolset , located at the bottom of the Mesh module toolbox.
Select the Node category, and click on Project in the Edit Mesh dialog box.
Use the angle method to select all the nodes on the bottom of the bottom-up extruded mesh, as shown in Figure 17–116; and then click Done in the prompt area.
Figure 17–116 Selecting the nodes to project.
Select the bottom face of the bottom-up region, and click Yes in the prompt area to project the nodes onto the face.

Completing the mesh for the bottom-up region

We will now create a final swept mesh to complete the mesh for the part.

Completing the mesh:

From the main menu bar, select MeshCreate Bottom-Up Mesh.
Select the bottom-up region.
Abaqus/CAE displays the Create Bottom-Up Mesh dialog box.
Select the Sweep method, and click Select to the right of Source side.
Select the two remaining unmeshed faces on the top of the part, as shown in Figure 17–117; and click Done in the prompt area.
Figure 17–117 Selecting the source side for the final bottom-up mesh.
Toggle on Connecting sides, and click Select. Rotate the part, and use the angle method to select the interior element faces from the outer swept mesh and the exterior element faces of the extruded mesh as shown in Figure 17–118.
Figure 17–118 Selecting the element faces as connecting sides.
Click Done in the prompt area to end selection.
Toggle on Target side, and click Select.
Abaqus/CAE prompts you to select a target side for the swept mesh.
Select the bottom face of the region.
Click Mesh in the Create Bottom-Up Mesh dialog box to create the mesh.

The part is now completely meshed with hexahedral elements, as shown in Figure 17–119.

Figure 17–119 The final meshed part.

Checking the association of the bottom-up mesh with the geometry

Before using the completed bottom-up mesh for an analysis, you should check the association between the region geometry and the bottom-up mesh elements. Loads, boundary conditions, and other attributes in Abaqus are applied to geometry, and they will not transfer correctly to the elements of a bottom-up mesh unless the mesh is correctly associated with the geometry. At minimum, you should check the association for areas of a bottom-up mesh where loads and boundary conditions are applied.

In most cases if you select a geometric feature, such as a face, to define the bottom-up mesh, Abaqus/CAE automatically associates the appropriate elements with that face. However, in cases where the geometry is not used, such as the extruded bottom-up mesh in the center of the example part, the elements are associated only with the region, not the nearby face where a load might be applied. (For more information, see “Mesh-geometry association,” Section 17.12.) The following procedure associates the elements on the bottom and front faces of the part with the geometric faces:

Associating the bottom-up mesh with the geometry:

From the main menu bar, select MeshAssociate Mesh with Geometry.
Select the bottom face of the bottom-up region, as shown in Figure 17–120.
The elements created in the final bottom-up meshing step are colored yellow because they were already associated when the face was used as the target side of the final bottom-up swept mesh. However, the elements in the semi-circular extruded mesh are not associated with the face.
Figure 17–120 Existing mesh associations on the bottom face.
Remove the top-down meshed cell that extends from the bottom-up region to the outer curved face of the part.
1. Select ToolsDisplay GroupsCreate.
  Abaqus/CAE displays the Create Display Group dialog box.
2. Select Cells from the item list, and click Edit Selection.
3. From the viewport, pick the top-down swept region that extends along the curved outer edge of the part and click Done in the prompt area.
4. In the Create Display Group dialog box, click the Remove button.
  Abaqus/CAE removes the selected cell from the viewport.
For more information, see Chapter 78, “Using display groups to display subsets of your model.”
Use the angle method to select all the faces on the bottom of the bottom-up region. When you are finished, all of the element faces on the bottom of the bottom-up region should be colored yellow, as shown in Figure 17–121.
Figure 17–121 Final mesh associations on the bottom face.
Note: If you did not remove the outer top-down meshed cell, use of the angle method would have selected the top-down element faces for association as well as the bottom-up faces, leading to an error message when you attempted to associate the faces.
Click Done in the prompt area to associate the selected elements' faces with the region face.

Associating the remainder of the bottom-up mesh

To fully associate the bottom-up mesh, you should verify and edit the association for the faces on the front side, the right side, and on each of the bounding edges and vertices in the bottom-up region. You associate edges and vertices the same way as you associated the element faces in the previous section, except that you select edges and element edges or vertices and nodes, respectively. Abaqus/CAE attempts to associate nodes with vertices and element edges with geometric edges based on proximity. If all the elements along an edge are associated with the faces bounded by that edge, Abaqus/CAE automatically associates the element edges with the geometric edge.

Once you have a part completely meshed and you have checked the association of the bottom-up mesh, you should save the model. Prior to running an analysis, you should also verify the quality of the mesh. Mesh verification helps ensure that there are no hidden problems, regardless of whether you created the mesh automatically (top-down) or used bottom-up techniques and mesh editing to construct the mesh. For more information on mesh verification, see “Verifying element quality,” Section 17.19.1.