Redefining region corners

Structured meshing patterns exist for regions with particular topologies. For example, Abaqus/CAE applies a particular structured pattern to quadrilateral regions and another pattern to pentagonal regions. In some cases, however, you can change the structured pattern assigned to a surface region by redefining the region's corners. You can redefine region corners only for surface regions to which the structured meshing technique has been assigned.

See Also
Controlling mesh characteristics
Using the Mesh module toolbox
Selecting objects within the viewport

Context:

If you click Redefine Region Corners in the Mesh Controls dialog box, you can select which corners of the region you want Abaqus/CAE to consider when creating the mesh. If you leave a corner unselected, Abaqus/CAE internally combines the edges on either side of the unselected corner into a single logical edge (though the actual topology of the region remains unchanged). For example, if you leave one corner of a pentagonal region unselected, Abaqus/CAE considers that region to have only four edges instead of five. As a result, the structured meshing pattern for quadrilateral regions will be applied to the region rather than the pattern for pentagonal regions. For more information, see Two-dimensional structured meshing.

A surface region can be meshed using the structured meshing technique only if the region is bounded by three to five logical sides. However, if the region contains virtual topology, Abaqus/CAE can apply structured meshing only if the region has four corners. As a result, to redefine the corners of a region with virtual topology, the region must be bounded by more than four corners, and you must select four of the existing corners.

  1. From the main menu bar, select MeshControls.

    Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.

    Tip: You can also click the tool, located in the Mesh module toolbox. (For more information, see Using the Mesh module toolbox.)

  2. If your part or assembly contains more than one region, select those regions whose corners you want to redefine and then press mouse button 2. The regions that you select should have three or more vertices.

    The Mesh Controls dialog box appears.

  3. Select Structured as the meshing technique if it is not already selected.

    The Redefine Region Corners button appears on the right side of the Mesh Controls dialog box.

  4. Click Redefine Region Corners.

    If you selected multiple regions, this procedure considers each of the selected regions in turn. (Abaqus/CAE skips selected regions that a structured pattern cannot be applied to or that contain three or fewer vertices.) The region currently being considered becomes highlighted in magenta. The currently selected corners for the region are highlighted in yellow.

  5. In the prompt area, select an option for determining region corners.

    • If you click Accept Highlighted, Abaqus/CAE accepts the currently highlighted corners. If multiple regions are selected, options are presented for the next region. If only one region is selected, the procedure is complete, and the Mesh Controls dialog box reappears.

    • If you click Select New, the currently selected vertices turn red. You must go on to the next step.

    • If you click Revert to Defaults, the default corners of the region are highlighted. You are prompted to select either Accept Highlighted or Select New, described above.

  6. If you clicked Select New in the previous step, select the vertices of the region that you want as region corners. You can select between three and five vertices.

    • ShiftClick to select a vertex without unselecting all the other vertices.

    • CtrlClick to unselect an individual vertex without unselecting all the other vertices.

    • When you have finished selecting vertices, click mouse button 2.

    Selected vertices are red, and unselected vertices are yellow.

    If multiple regions are selected, the procedure starts over with the next region. If only one region is selected, the procedure is complete and the Mesh Controls dialog box reappears.