Inertia Relief

Allows the simulation of unconstrained structures. Typical applications are an airplane in flight, suspension parts of a car, or a satellite in space.

With inertia relief, the applied loads are balanced by a set of translational and rotational accelerations. These accelerations provide body forces, distributed over the structure in such a way that the sum total of the applied forces on the structure is zero. This provides the steady-state stress and deformed shape in the structure as if it were freely accelerating due to the applied loads. Boundary conditions are applied only to restrain rigid body motion. Because the external loads are balanced by the accelerations, the reaction forces corresponding to these boundary conditions are zero.

This calculation is automated.

Inertia relief boundary conditions may be defined in the Bulk Data section of the input deck or they may be determined automatically by the solver.

Use SUPORT Entries

  • PARAM,INREL,-1 is used to activate inertia relief.
  • The SUPORT and SUPORT1 Bulk Data Entries are used to define up to six reaction degrees of freedom of the free body.
  • SUPORT entries will be used in all relevant subcases and therefore do not need to be referenced in the Subcase Information section.
  • SUPORT1 entries need to be referenced by a SUPORT1 data selector statement for use within a subcase.

Automatic Support Generation

Up to six rigid body modes:
  • Inertia relief boundary conditions may be generated automatically by using PARAM,INREL,-2.
Greater than six rigid body modes:
  • Inertia relief boundary conditions may be generated automatically by using PARAM,INREL,-2.
  • The METHOD parameter on PARAM,INREL can reference the ID of EIGRL or EIGRA entry.
  • Eigenvalue subcases are internally generated to calculate the rigid body modes, inertial loads, and support points.

In OptiStruct, inertia relief can be applied to linear static, nonlinear static analyses, and modal frequency response analyses. For Nonlinear static analysis with contact, by default, only freeze contact is supported with inertia relief. If non-freeze contact is present, PARAM,IR4NLCON,YES can be used to allow the model to run with inertia relief. A static case with inertia relief cannot be referenced in a linear buckling analysis. Inertia relief is meaningless in normal modes analysis.