Defining MPC constraints

You use an MPC constraint to constrain the motion of slave nodes of a region to the motion of a point. You can create an MPC constraint by specifying a control point and a region composed of nodes, edges, and surfaces. For detailed information about multi-point constraints, see General multi-point constraints.

  1. From the main menu bar, select ConstraintCreate.

    Tip: You can also create a multi-point 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 MPC Constraint, then click Continue.

  3. Select a point to define the constraint control point using one of the following methods:

    • Use the mouse to select a point in the viewport.

      Tip: The Select the Entity Closest to the Screen tool in the Selection toolbar is toggled off by default. If you make an ambiguous selection, Abaqus/CAE highlights the point and displays a description of the point in the lower left corner of the viewport. Use the Next and Previous buttons to cycle through the possible selections, and click OK to confirm your selection.

      (For more information, see Selecting objects within the current viewport.) Click mouse button 2 to indicate that you have finished selecting.

      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 the control point from a geometry region.

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

    • Use an existing set to define the region. On the right side of the prompt area, click Sets. Select an existing set 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 on the right side of the prompt area.

    The point that you select becomes highlighted in red in the viewport.

  4. Select the region for the slave nodes. Use one of the following methods to select the region:

    • Use the mouse to select a region in the viewport. (For more information, see Selecting objects within the current viewport.) The region that you select can span multiple part instances. Click mouse button 2 to indicate that you have finished selecting.

      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 the region from a native or orphan mesh selection.

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

    • Use an existing set to define the region. On the right side of the prompt area, click Sets. Select an existing set from the Region Selection dialog box that appears and click Continue.

      Note:

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

    The region that you select becomes highlighted in magenta in the viewport.

    The constraint editor appears.

  5. From the editor, select the MPC type.

    • Select Beam to define a rigid beam connection to constrain the displacement and rotation of each slave node to the displacement and rotation of the control point.

    • Select Tie to make all active degrees of freedom equal at each slave node and the control point.

    • Select Link to define a pinned rigid link between each slave node and the control point.

    • Select Pin to define a pinned joint between each slave node and the control point.

    • Select Elbow to constrain nodes of ELBOW31 or ELBOW32 elements together (see Pipes and pipebends with deforming cross-sections: elbow elements).

    • Select User-defined to define a multi-point constraint in user subroutine MPC (for Abaqus/Standard). See the following sections for more information:

  6. If you selected a user-defined MPC type, do the following:

    1. Choose the coding mode for user subroutine MPC.

      • Choose DOF-by-DOF if you want each call to the user subroutine to constrain one individual degree of freedom.

      • Choose Node-by-Node if you want each call to the user subroutine to impose a set of constraints all at once.

    2. In the Constraint type field, enter an integer value to be used in the user subroutine to distinguish between different constraint types. The default value is 0.

  7. If you want to change the coordinate system (CSYS) for the coupling constraint, click and use one of the following methods:

    • Select a predefined datum coordinate system by name.

      1. From the prompt area, click Datum CSYS List to display a list of datum coordinate systems.

      2. Select a name from the list, and click OK.

    • Select a predefined coordinate system in the viewport.

      Tip: The tool in the Selection toolbar is toggled off by default. For coordinate systems with coincident origins, when you cycle through all of the possible selections, Abaqus/CAE highlights the coordinate system and displays the description of the coordinate system in the viewport.

    • Click Use Global CSYS from the prompt area to use the global coordinate system.

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