Defining rigid body constraints

You can create a rigid body constraint by specifying the regions that you want to include in the rigid body and by specifying a rigid body reference point. For detailed information about rigid bodies, see Rigid body definition.

Related Topics
Understanding constraints
In Other Guides
Rigid body definition

  1. From the main menu bar, select ConstraintCreate.

    Tip: You can also create a rigid body constraint using the tool in the Interaction module toolbox.

  2. In the Create Constraint dialog box that appears, do the following:

    1. Name the constraint. For more information about naming objects, see Using basic dialog box components.
    2. From the Type list, select Rigid Body, and then click Continue.

    The constraint editor appears.

  3. From the editor, select all of the regions that you want to include in the rigid body.

    1. Select one of the following from the Region type list:

      • Select Body if you want to include the elements of a geometric region or orphan elements in the rigid body.

      • Select Pin to include nodes that will have only translational degrees of freedom associated with the rigid body.

      • Select Tie to include nodes that will have both translational and rotational degrees of freedom associated with the rigid body.

      • Select Analytical Surface to include an analytical surface in the rigid body.

    2. After you select a region type, click on the right side of the editor.
    3. Select a region of the assembly to associate with the Region type category selected in the previous step. Use one of the following methods to select the region:

      • Use an existing set or surface to define the region. On the right side of the prompt area, click Sets or Surfaces. Select an existing set or surface from the Region Selection dialog box that appears, 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 Select in Viewport or Sets or Surfaces on the right side of the prompt area.

      • Use the mouse to select the region in the viewport. (For more information, see Selecting objects within the current viewport.)

        If the model contains a combination of mesh and geometry, click one of the following from the prompt area:

        • Click Geometry if you want to select a geometry region.

        • Click Mesh if you want to select nodes from a native or orphan mesh selection.

        You can use the angle method to select a group of faces or edges from geometry or a group of element faces from a mesh. For more information, see Using the angle and feature edge method to select multiple objects.

    4. To remove a region type from the rigid body, select that region type, and then click on the right side of the editor.

  4. Repeat Step 3 as often as necessary to select all of the regions that you want to include in the rigid body.

  5. Select the rigid body reference point:

    1. In the bottom half of the editor, click .
    2. Use one of the techniques described above to select a vertex or node to serve as the rigid body reference point. For more information, see The Reference Point toolset.”

  6. Toggle on Adjust point to center of mass at start of analysis if you want Abaqus to reposition the rigid body reference point at the calculated center of mass of the rigid body.

  7. Toggle on Constrain selected regions to be isothermal to specify an isothermal rigid body for a fully coupled thermal-stress analysis.

  8. Click OK to save your constraint definition and to close the editor.