Element types can be assigned to the following:
A region selected from geometry-based parts or part instances. The part instances must have come from parts that you created in the Part module or from parts that you imported.
A set that refers to a region selected from geometry-based parts or part instances. The set can also refer to a skin reinforcement.
An element or an element set from an orphan mesh part.
All regions from geometry-based parts or part instances and all elements from an orphan mesh part have default element type assignments. These assignments depend on the kind of part to which the region or element belongs. You can view and change the ABAQUS element types that are assigned using the Element Type dialog box, which you can display by selecting Mesh
Element Type. For example, the Element Type dialog box for a two-dimensional region is shown in Figure 17–20.
At the top of the dialog box, you enter your preferences for element library, geometric order, and family. Then, you select a specific element type by clicking the tabs in the bottom half of the dialog box and choosing from the options that appear. The dialog box can contain from one to three tabs depending on the dimensionality of the selected region or regions:
The Line tab allows you to choose an applicable element type and assign it to one-dimensional mesh elements in the region.
The Quad and Tri tabs allow you to choose an applicable element type and assign it to two-dimensional mesh elements in the region.
The Hex, Wedge, and Tet tabs allow you to assign three-dimensional element types to the three-dimensional mesh elements in the region.
For example, in Figure 17–20 the options for a linear shell element from the ABAQUS/Standard element library are selected. After clicking the Quad tab, reduced integration and finite membrane strains are selected. The name and a brief description of the quadrilateral shell element that meets all of these criteria appear at the bottom of the tabbed page.
The Tri tab in this dialog box is shown in Figure 17–21.
The name and a brief description of the triangular shell element that meets all of the criteria specified in the dialog box appear at the bottom of the Tri tabbed page in Figure 17–21. If the selected region in this example happens to contain a combination of triangular and quadrilateral mesh elements:The quadrilateral mesh elements are assigned the S4R element type.
The triangular mesh elements are assigned the S3 element type.
If the region contains only quadrilateral elements, all of the elements are assigned the S4R element type.
For detailed, step-by-step instructions for assigning element types to a mesh region, see “Associating ABAQUS elements with mesh regions,” Section 17.15.10. For lists of the element types that are available, see Section I.1, “ABAQUS/Standard Element Index,” of the ABAQUS Analysis User's Manual, and Section I.2, “ABAQUS/Explicit Element Index,” of the ABAQUS Analysis User's Manual. You can select most of these elements through the Element Type dialog box. “What kinds of elements must be generated outside the Mesh module?,” Section 17.5.2, describes the elements that cannot be selected.
