Does ANSYS re-form the system matrices at each time step?

The direct solvers (frontal and sparse) contain internal logic to determine whether or not the matrices need to be reformed. This feature is turned on by default, and rarely needs user intervention.

In a static analysis, the stiffness matrix may need to be reformed if, for example, nonlinearities are present (large deflection, material nonlinearities, contact, etc) or if boundary conditions change.

In a transient analysis, the coefficient matrix given by (a0[M]+a1[C]+[K]) in Theory Reference equation (17-11), which is sometimes referred to as the "dynamic stiffness," may need to be reformed if any item mentioned for static analysis is present or if the time-step size changes, since the a0 and a1 terms contain delta-times.

You can easily tell whether or not new matrices were formed by checking the output file for "NEW TRIANG MATRIX" or "OLD TRIANG MATRIX" messages; for example, when large deflection (NLGEOM) is turned off in a transient analysis, you may see the same matrices used throughout the analysis if the time step time does not change.

If you want to probe a little further, take a look at the KUSE command (not intended for general use). You can run your transient analysis with NLGEOM,OFF, then try it with KUSE,-1, which will force matrix regeneration. It might be interesting to compare this to the case with NLGEOM,ON and KUSE,0 (default).

Please also see Theory Reference section 13.3 for additional information on the reuse of matrices.

Show Form
No comments yet. Be the first to add a comment!