Refining a planar, triangular mesh

You can refine a planar, triangular mesh with or without a specified global element size.

This task shows you how to:

Related Topics
What can I do with the Edit Mesh toolset?

Context:

Select MeshEdit from the main menu bar to refine a planar, triangular mesh. You can remesh the part using the following methods:

With a specified global element size

Before you remesh the part, you have the option of assigning a target element size to the entire part. You can then remesh the part, and the density of the new mesh reflects the new target element size. For example, when the part in Figure 3 is remeshed with a global element size of 15.0, Figure 1 shows the resulting mesh.

Figure 1. A global element size of 15.0.

Figure 2 shows the part remeshed with a global element size of 8.0.

Figure 2. A global element size of 8.0.

Without a specified global element size

If no global element size is specified, Abaqus/CAE maintains the edges of the elements along the boundary of the part while improving the mesh quality in the interior of the part. The resulting mesh topology is different from the original mesh topology. For example, Figure 3 shows a distorted mesh.

Figure 3. A distorted mesh.

When the part is remeshed, the quality of the mesh improves dramatically, as shown in Figure 4.

Figure 4. The part is remeshed without specifying a global element size.

Refine a planar, triangular mesh with a specified global element size

  1. Enter the Mesh module.

  2. From the Object field in the context bar, select Part and select a part that contains only orphan mesh elements from the list.

    Tip: To refine the orphan elements within a hybrid part, suppress the geometric features and resume them after completing the refinement operation.

  3. From the main menu bar, select MeshEdit.

    Abaqus/CAE displays the Edit Mesh dialog box.

    Tip: You can also display the Edit Mesh dialog box using the tool, located at the bottom of the Mesh module toolbox.

  4. In the dialog box, choose Refinement from the Category field.

  5. From the Method list, select Set size.

  6. In the prompt area, type the global element size of your choice, and press Enter.

    Abaqus/CAE displays a circle that indicates what the size of the elements will be after you remesh the part.

  7. From the Method list, select Remesh.

  8. From the buttons that appear in the prompt area, click Yes.

    Abaqus/CAE attempts to refine the mesh. If you make a mistake while refining the mesh, click Undo in the Edit Mesh dialog box to undo the refinement.

Refine a planar, triangular mesh without a specified global element size

  1. Enter the Mesh module.

  2. From the Object field in the context bar, select Part and select a part that contains orphan mesh elements from the list.

    Tip: To refine the orphan elements within a hybrid part, suppress the geometric features and resume them after completing the refinement operation.

  3. From the main menu bar, select MeshEdit.

    Abaqus/CAE displays the Edit Mesh dialog box.

    Tip: You can also display the Edit Mesh dialog box using the tool, located at the bottom of the Mesh module toolbox.

  4. In the dialog box, choose Refinement from the Category field.

  5. From the Method list, select Remove size.

  6. From the Method list, select Remesh.

  7. From the buttons that appear in the prompt area, click Yes.

    Abaqus/CAE attempts to refine the mesh. If you make a mistake while refining the mesh, click Undo in the Edit Mesh dialog box to undo the refinement.