Defining tie constraints

A tie constraint ties two separate surfaces together so that there is no relative motion between them. This type of constraint allows you to fuse together two regions even though the meshes created on the surfaces of the regions may be dissimilar. You can define a tie constraint between edges of a wire or between faces of a solid or shell. For more information, see Understanding constraints, and Mesh Tie Constraints.

See Also
Understanding constraints

Context:

If you are creating multiple tie constraints, you may want to use the automatic contact detection tool. This tool automates the process of selecting surfaces and allows you to create multiple constraints simultaneously. For more information, see Using contact and constraint detection.

  1. From the main menu bar, select ConstraintCreate.

    Tip: You can also create a tie 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 Tie, then click Continue.
  3. Select the main surface.
    1. In the prompt area, select one of the following:

      • Select Surface if you want to select a named surface.

      • Select Node Region if you want to select a region from which to create a node-based surface.

    2. Use one of the following methods to select the main surface:

      • Use an existing surface to define the region. On the right side of the prompt area, click Surfaces. Select an existing surface name 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 Surfaces on the right side of the prompt area.

      • Use the mouse to select a region in the viewport. (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 surface or vertex from a geometry region.

        • Click Mesh if you want to select the surface or node 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.

      The main surface that you select becomes highlighted in red in the viewport.

  4. Select the secondary surface.
    1. In the prompt area, select one of the following:

      • Select Surface if you want to select a surface.

      • Select Node Region if you want to select a region from which to create a node-based surface.

    2. Use one of the same methods described in the previous step to select the secondary surface or region.

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

      The constraint editor appears.

  5. The Switch Surfaces option allows you to interchange your main and secondary surface selections without having to start over. The Switch Surfaces icon is available only when the main and secondary regions are the same type—both surfaces or both node-based regions.
  6. From the editor, select the Discretization method.

    • Select Analysis default to use the default discretization method: surface-to-surface for Abaqus/Standard and node-to-surface for Abaqus/Explicit.

    • Select Node to surface to generate the tie coefficients according to the interpolation functions at the point where the secondary node projects onto the main surface.

    • Select Surface to surface to generate the tie coefficients such that stress accuracy is optimized for the specified surface pairing.

  7. Toggle on Exclude shell element thickness if you want to ignore shell thickness effects in calculations involving position tolerances and adjustments for initial gaps.
  8. Choose one of the following Position Tolerance methods:

    • Use computed default. Abaqus determines the nodes to be tied using the default position tolerance. For more information, see Mesh Tie Constraints.

    • Specify distance. You can specify an absolute distance from the main surface within which all nodes on the secondary surface to be tied must lie.

  9. Toggle on Adjust secondary surface initial position if you want Abaqus to move all the nodes of the secondary surface onto the main surface in the initial configuration.
  10. Toggle on Tie rotational DOFs if applicable if you want Abaqus to constrain the rotational degrees of freedom that exist on both main and secondary surfaces.
  11. If desired, you can specify a value for the constraint ratio. You must toggle off Tie rotational DOFs if applicable to make the constraint ratio option available.
  12. Click OK to save your constraint definition and to close the editor.