Assigning a section

Context:

You can also use the Section Assignment Manager to view, create, edit, suppress, resume, and delete section assignments. For more information, see Managing section assignments. You can use the Query toolset to verify that you have assigned the correct section to a selected region. For more information, see Using the Query toolset to obtain assignment information.

You can create overlapping section assignments anywhere in your model except for a region that contains Eulerian parts. Eulerian parts can be assigned only a single section assignment, and you cannot apply a second section assignment to an Eulerian part, even when its original section assignment is suppressed.

When you import a mesh from an input file, some section properties associated with that mesh may also be imported; in these cases it may be unnecessary to assign section properties to the part. For more information, see Importing a model from an Abaqus input file.

If the part to which you want to assign a section is not visible in the current viewport, click the name of the desired part in the Part list located in the context bar.
The part that you select appears in the current viewport.
From the main menu bar, select AssignSection.

Tip: You can also click Create in the Section Assignment Manager or select the tool in the Property module toolbox.

Select the regions of the part from the viewport, and click mouse button 2 to indicate you have finished selecting. (For more information, see Selecting objects within the viewport.) If an Eulerian part is in the current viewport, Abaqus/CAE automatically selects the entire part.

Tip: You can limit the types of objects that you can select in the viewport by using the tools in the Selection toolbar. See Using the selection options for more information.

If you select Skins as the object type, you can assign the section to the entire skin or to one or more of its faces. From the prompt area, select (pick entire skin) or (pick partial skin), then make your selection in the viewport. If the selected part has multiple skins, Abaqus/CAE will display the ambiguous picking options in the prompt area while you make your selection.

If you select Stringers as the object type, you can assign the section to the entire stringer or to one or more of its edges. From the prompt area, select (pick entire stringer) or (pick partial stringer), then make your selection in the viewport. If the selected part has multiple stringers, Abaqus/CAE will display the ambiguous picking options in the prompt area while you make your selection.

If you would rather select from a list of existing sets, do the following:

Click Sets on the right side of the prompt area.
Abaqus/CAE displays the Region Selection dialog box containing a list of available part sets and element sets.
Select the desired set, and click Continue.

Note: The default selection method is based on the selection method you most recently employed. To revert to the other method, click the button—Select in Viewport or Sets—on the right side of the prompt area.

An Edit Section Assignment dialog box appears. This dialog box contains a list of existing sections that can be assigned to the selected region or set. For example, if you selected a solid region, any existing solid sections appear in the Edit Section Assignment dialog box. In addition, the dialog box contains a Create Section button and the section type, material, and region of the displayed section.

In the Edit Section Assignment dialog box, select the section of interest and click OK.

Abaqus/CAE assigns the selected section to the part or set and colors the selected region green to indicate that the region has a section assignment. If there are overlapping section assignments on the region, Abaqus/CAE colors the region yellow.

Note: The order of assignments may be relevant; when section assignments overlap, the last assignment will take precedence.
Assign a section thickness:

From section

Use the thickness defined in the section definition.

From geometry

Use the thickness of the geometric section.
If you assign a homogeneous or a composite section to a shell, you can define the method used for the Shell Offset. Click the arrow to the right of the Definition field, and select the option of your choice from the list that appears:
- Select Middle surface, Top surface, or Bottom surface to represent the reference surface.
- Select Specify value, and enter a positive or negative distance (as a fraction of the shell thickness) from the midsurface to the reference surface of the shell in the Offset ratio field.
  
  A positive offset will generate nodes and elements closer to the top surface of the shell, and a negative offset will generate them closer to the bottom surface. Offsets greater than ±0.5 will cause the nodes to be beyond the surface of the shell.
- Select an existing scalar discrete field that defines an offset that is varying spatially across the section. Abaqus/CAE allows you to select only valid discrete fields, which, for an offset, are scalar discrete fields applied to elements. This option is valid only for an Abaqus/Standard analysis. Alternatively, you can click to create a new discrete field. (See The Discrete Field toolset for more information.)
- Select From geometry to have Abaqus/CAE calculate the offset from the thickness defined on the geometry. This option is the default if From geometry is selected in the Thickness field. You cannot use this option to calculate the offset in an Abaqus/Explicit analysis.
If you want to assign sections to additional regions, repeat Steps 3 and 4. When you have finished assigning sections, use one of the following methods to exit the section assignment mode:
- If you are selecting regions of the part from the viewport, click mouse button 2 or click Done in the prompt area.
- If you are selecting preexisting sets from the Region Selection dialog box, click Cancel to close the dialog box, then click mouse button 2 or click Done in the prompt area.