When the Mesh defaults color mapping is selected, the color of a region in the Mesh module indicates the meshing technique currently assigned to that region. The color coding is as follows:

See “Structured meshing and mapped meshing,” Section 17.8; “Free meshing,” Section 17.9; and “Swept meshing,” Section 17.10, for information about each meshing technique. See Chapter 51, “Color coding geometry and mesh elements,” for more information about color mappings.

In many cases ABAQUS/CAE can use more than one technique to mesh a region; in these cases you can either accept the default technique, or you can use the Mesh Controls dialog box to select an alternative technique. In addition, you can change which meshing techniques are valid for a region by adding partitions to the region or by assigning a different element shape to the region. For example, if you change the element shape assignment of an unmeshable three-dimensional part instance from hexahedra to tetrahedra, the part instance becomes meshable using the free-meshing technique. For more information, see “Why partition in the Mesh module?,” Section 17.6.3.

The default meshing technique for two-dimensional models is the free meshing technique. If you are not satisfied with the quality of the mesh generated by the free meshing technique, you can assign structured meshing to the simpler regions of your model. You can also assign structured meshing to the simpler regions if you prefer a more regular grid-like mesh pattern. However, if your model is large and complex, identifying the simple regions where structured meshing is applicable can be a time-consuming process. To make the process faster, you can apply the structured meshing technique to the entire model, and ABAQUS/CAE will do the following:

If ABAQUS/CAE removed any faces from your selection, they are colored pink to indicate that they will be meshed using free meshing. Remaining faces are colored green to indicate that ABAQUS/CAE will mesh them using structured meshing.

For example, Figure 17–32 shows a shell model of an electrical connector. The user attempted to assign structured meshing to the entire assembly, and ABAQUS/CAE removed the indicated faces from their selection.

If you are meshing a solid model, you must select one or more cells and use the Mesh Controls dialog box to determine whether the structured technique can be applied to those cells.

For detailed information on controlling the mesh technique and element shape assigned to a region, see the following sections: