Assigning an Abaqus element type

In this section you will assign a particular Abaqus element type to the model. Although you will assign the element type now, you could also wait until after the mesh has been created.

Context:

Two-dimensional truss elements will be used to model the frame. These elements are chosen because truss elements, which carry only tensile and compressive axial loads, are ideal for modeling pin-jointed frameworks such as this overhead hoist.

  1. In the Model Tree, expand the Frame item underneath the Parts container if it is not already expanded. Then double-click Mesh in the list that appears.

    Abaqus/CAE switches to the Mesh module. The Mesh module functionality is available only through menu bar items or toolbox icons.

  2. From the main menu bar, select MeshElement Type.
  3. If you created the set named all while assigning section properties, click Sets in the right side of the prompt area and select all from the Region Selection dialog box. Otherwise, drag the mouse to create a box that selects the entire frame as the region to be assigned an element type and click Done in the prompt area when you are finished.

    The Element Type dialog box appears.

  4. In the dialog box, select the following:

    • Standard as the Element Library selection (the default).

    • Linear as the Geometric Order (the default).

    • Truss as the Family of elements.

  5. In the lower portion of the dialog box, examine the element shape options. A brief description of the default element selection is available at the bottom of each tabbed page.

    Since the model is a two-dimensional truss, only two-dimensional truss element types are shown on the Line tabbed page. A description of the element type T2D2 appears at the bottom of the dialog box. Abaqus/CAE will now associate T2D2 elements with the elements in the mesh.

  6. Click OK to assign the element type and to close the dialog box.
  7. In the prompt area, click Done to end the procedure.