Constraints

Constraints are defined on the analysis degrees of freedom between regions of a model. The following section discusses the constraints available in Nonlinear Structural Analysis:

Creating Rigid Body Constraints: Constrains the motion of regions of a part so that the relative positions of points in the region remain constant throughout the analysis, prohibiting deformation.

Creating Rigid Body Constraints

A rigid body constraint allows you to constrain the motion of selected parts and points so that the relative positions of points in the body remain constant throughout the analysis, prohibiting deformation. A rigid body will, therefore, have three free translational and three free rotational motions; these motions can be prescribed by applying boundary conditions to the rigid body. If no boundary conditions are applied, the body will behave as a free rigid body.

Rigid bodies can consist of three-dimensional bodies, groups of points, or a combination of bodies and points. The points can be connected to other, deformable bodies. Points that are part of a rigid body can be defined as either tie nodes or pin nodes. A tie node transmits both translational and rotational degrees of freedom to any body to which it is attached. A pin node transmits only translational degrees of freedom to any body to which it is attached. Figure 7–1 illustrates the difference between the two node types. Points on either end of the octagonal rigid body are connected to deformable bodies. When the rigid body is rotated, the deformable bodies attached to tie nodes rotate as well, while the deformable bodies attached to pin nodes displace while retaining their rotational orientation.

Figure 7–1 Rigid body with tie node and pin node connections.

You can specify the handler, or reference point, for the rigid body constraint by selecting a vertex or by selecting a point group (containing a single point). You can instruct Nonlinear Structural Analysis to redefine the handler point at a point corresponding to the calculated center of mass of the rigid body during the analysis; any boundary conditions applied to the handler point will then act on the rigid body's center of mass. If you do not specify a handler point, Nonlinear Structural Analysis creates it at the approximate centroid of the selected parts; Abaqus moves the handler from the approximate centroid to the calculated center of mass during the analysis.

Rigid body constraints are available only in the Nonlinear Structural Analysis workbench.

This task shows you how to create a rigid body constraint.

  1. Click the Rigid Body Constraint icon .

    The Rigid Body Constraint dialog box appears. A Rigid Body Constraint object appears in the specification tree under the Connections objects set for the Initialization step, and a Rigid Body Constraint Connection Mesh appears under the Nodes and Elements objects set.

  2. You can change the identifier of the constraint by editing the Name field.

  3. If desired, select the part or parts to constrain in the window or in the specification tree.

    The Support field is updated to reflect your selection.

  4. If desired, select vertices or points to act as pin nodes in the rigid body.

    The Pin points support field is updated to reflect your selection.

  5. If desired, select vertices or points to act as tie nodes in the rigid body.

    The Tie points support field is updated to reflect your selection.

  6. If desired, select a vertex or point group to represent the handler point.

    The Handler field is updated to reflect your selection.

  7. To move a selected handler point to the center of mass of the rigid body during the analysis, toggle on Move to center of mass.

  8. Click OK in the Rigid Body Constraint dialog box.

    Symbols representing the rigid body constraint appear on the corresponding parts.