NASTRAN Inertia Relief

Inertia relief is an option in NASTRAN that allows you to simulate unconstrained structures in a static analysis.

One example in which this can be used is an object in flight.  Static analysis via the finite element method requires the model to be constrained in all directions.  If the model being analyzed is not fully constrained, singularities occur in the stiffness matrix and the model will either not solve, or the results will be invalid.

Inertia relief utilizes the inertia of the structure to create a state of static equilibrium, allowing the model to be solved.  To invoke inertia relief, you must provide a SUPORT bulk data entry that lists the unconstrained degrees of freedom in the model (*note: if automatic inertia relief is selected, NASTRAN performs this operation for you).  One way to describe the SUPORT entry is if you hold the model at this point in the directions specified, there is no possible rigid body motion (the model is constrained).

When inertia relief is specified, a PARAM,GRDPNT,x entry is required (*note: If automatic inertia relief is selected, NASTRAN does not use the PARAM,GRDPNT option, the basic origin is used).

NASTRAN calculates the forces that result from rigid body accelerations about this point in the directions specified in the SUPORT entry.  The summation of all applied loads in these directions is then calculated.  NASTRAN then applies accelerations to the structure in the appropriate directions to “balance” the applied loadings.  This results in a state of static equilibrium (i.e. the summation of all applied loads and induced accelerations is 0.0).

NASTRAN next constrains the SUPORT degrees of freedom to a displacement of 0.0 and calculates the displacement of all other grid points with relation to the SUPORT grid point.