25.2.9 Connector failure behavior

Products: ABAQUS/Standard  ABAQUS/Explicit  ABAQUS/CAE  



Connector failure behavior:

  • can be defined in any connector with available components of relative motion;

  • can be used to fail all or specified components of relative motion if a specified criterion is met;

  • can be triggered if either a connector relative motion or connector force in a specified component is outside a specified range; and

  • can be replaced in most cases by the more sophisticated connector damage initiation/evolution behavior (see Connector damage behavior, Section 25.2.7).

Defining connector failure behavior

A typical connector might have pieces that break if a relative motion component, force, or moment becomes too large. ABAQUS provides a way to define which components of relative motion will break and the criteria used to release these components. You can select the component of relative motion on which the failure criterion is based.

Connector failure can be used to specify connector behavior based on constrained as well as available components of relative motion. Limit values for force or moment can be specified for all components of relative motion involved in the connection. In addition, for connectors with available components of relative motion, limit values can be specified for the relative positions corresponding to an available component.

If the failure criterion specified for the selected component of relative motion is met, either all components of relative motion fail or a single available component fails. By default, all components of relative motion are released upon meeting the failure criterion. In this case the connector element will have no effect on the analysis from that point on. All nodal force contributions from the connector element will be removed during the increment when the failure criterion is met.

Input File Usage:           Use the following options to define connector failure:
RELEASE=ALL or component number


Interaction module: connector section editor: AddFailure: Components: component or components, Release: All or Specify component

Viscous damping in ABAQUS/Standard

In ABAQUS/Standard the sudden release of the failed connection may lead to convergence problems. To avoid convergence problems, you can add viscous damping to the components. Damping forces in the component are calculated as , where is the user-defined damping coefficient and is the velocity of the failed component. Viscous damping is applied only if a selected available component of relative motion is released.

Input File Usage:           Use the following options to add viscous damping to failed components in ABAQUS/Standard:

ABAQUS/CAE Usage: Viscous regularization is not supported in ABAQUS/CAE.


In the example in Figure 25.2.9–1 assume that the shock absorber pulls apart if the tensile force in the shock exceeds 800.0 units of force.

Figure 25.2.9–1 Simplified connector model of a shock absorber.

, , , 800.0


The ABAQUS output variables available for connectors are listed in ABAQUS/Standard output variable identifiers, Section 4.2.1, and ABAQUS/Explicit output variable identifiers, Section 4.2.2. The following output variables are of particular interest when defining failure in connectors:


Flags for connector failure status.


Energy dissipated by viscous damping added to failed components.