Getting Started with ABAQUS  


B.5 Defining and assigning section properties

You define the properties of a part through sections. After you create the section, you can use one of the following two methods to assign the section to the part in the current viewport:

  • You can simply select the region from the part and assign the section to the selected region.

  • You can use the Set toolset to create a homogeneous set containing the region and assign the section to the set.

For the cantilever beam tutorial you will create a single homogeneous solid section that you will assign to the beam by selecting the beam from the viewport. The solid section will contain a reference to the material Steel that you just created.


B.5.1 Defining a homogeneous solid section

A homogeneous solid section is the simplest section type that you can define; it includes only a material reference and a plane stress/plane strain thickness.

To define the homogeneous solid section:

  1. In the Model Tree, double-click the Sections container to create a section.

    The Create Section dialog box appears.

  2. In the Create Section dialog box:

    1. Name the section BeamSection.

    2. In the Category list, accept Solid as the default category selection.

    3. In the Type list, accept Homogeneous as the default type selection.

    4. Click Continue.

      The Edit Section dialog box appears.

  3. In the dialog box:

    1. Accept the default selection of Steel for the Material associated with the section.

    2. Accept the default value of 1 for the Plane stress/strain thickness.

    3. Click OK.

For information on related topics, click the following item:


B.5.2 Assigning the section to the cantilever beam

The section BeamSection must be assigned to the part.

To assign the section to the cantilever beam:

  1. In the Model Tree, expand the branch for the part named Beam by clicking the “” symbol to expand the Parts container and then clicking the “” symbol to expand the Beam item.

  2. Double-click Section Assignments in the list of part attributes that appears.

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

  3. Click anywhere on the beam to select the region to which the section will be applied.

    ABAQUS/CAE highlights the entire beam.

  4. Click mouse button 2 in the viewport or click Done in the prompt area to accept the selected geometry.

    The Edit Section Assignment dialog box appears containing a list of existing sections.

  5. Accept the default selection of BeamSection as the section, and click OK.

    ABAQUS/CAE assigns the solid section to the beam, colors the entire beam aqua to indicate that the region has a section assignment, and closes the Edit Section Assignment dialog box.

Note the following key point:

  • When you assign a section to a region of a part, the region takes on the material properties associated with the section.

For information on related topics, click any of the following items: