To associate particular ABAQUS elements with mesh regions or with an orphan mesh, select Mesh
Element Type from the main menu bar. Then select those regions whose element type you want to assign, and make the assignment using the Element Type dialog box that appears.
You can use the dialog box to specify ABAQUS element settings for all the element shapes that could conceivably appear in the regions you select, even if the regions currently contain only a few different element shapes. For example, even though a selected region may contain only quadrilateral elements, you can associate an element type with other shapes, too, such as triangles.
The element type setting behaves like a feature. For example, if you assign element types to a region and then later partition that region into several more regions, the new regions will inherit the element type settings of the original parent region.
To associate ABAQUS elements with mesh regions:
From the main menu bar, select MeshElement Type.
ABAQUS/CAE displays prompts in the prompt area to guide you through the procedure.
Tip:
You can also choose element types using the 
tool, located in the Mesh module toolbox. (For more information, see “Using the Mesh module toolbox,” Section 17.13.)
If your assembly contains both orphan meshes and native part instances,
click Mesh in the prompt area to assign an element type to an orphan mesh, or
click Geometry in the prompt area to assign an element type to native geometry.
If you are selecting from multiple regions of ABAQUS/CAE native geometry or if you are selecting elements from a part imported from an output database, use the following selection techniques:
ABAQUS/CAE native geometry
Use the mouse to select the desired regions in the viewport, and then click mouse button 2 when your selection is complete.
You can select only regions from parts of the same type; for example, you cannot select both a rigid surface and a deformable body. Likewise, the regions that you choose must have the same dimensionality.
A part imported from an output database
Use the mouse to select the desired elements of the part, and then click mouse button 2 when your selection is complete.
Alternatively, you can click Sets on the right side of the prompt area. A dialog box appears with a list of all of the elements sets associated with the meshed part. Select the element set of your choice and then click Continue. For information on creating sets, see Chapter 48, “The Set and Surface toolsets.”
All elements that you select, regardless of the selection method, must be of the same order. In addition, the elements must belong to parts of the same type.
The Element Type dialog box appears.
In the upper left corner of the dialog box, select the Element Library option of your choice.
Select Standard to choose from the list of ABAQUS/Standard elements, or select Explicit to choose from the list of ABAQUS/Explicit elements.
Select the Geometric Order of your choice: Linear (first order) or Quadratic (second order).
From the Family list on the right side of the dialog box, select an appropriate element family for the type of analysis you will perform on the model. For example, if you plan to do a heat transfer analysis, select the Heat Transfer family.
If you have not yet assigned ABAQUS element types to the region, the name of a default element for the element library, geometric order, and family that you specified appears in the lower half of the dialog box.
Note: You can set the element type corresponding to only a single family. For example, you cannot set the element type for linear triangles in both the plane strain and heat transfer families; you must select either heat transfer or plane strain. If, after setting element types for one family, you switch to another family, the settings for the first family are lost.
Choose the ABAQUS element type of your choice for each element shape.
Click the tab corresponding to the element shape of interest.
Select the element characteristics of your choice.
The name of the ABAQUS element that meets all your criteria appears at the bottom of the tabbed page with a brief description.
Click OK to commit your element type assignments, or click Defaults and then OK to return all element settings to their default values.
The element types are changed according to your specifications.
To set element types for additional regions, repeat this procedure starting from Step 2.
