Hello!,
A contact condition can be included in a normal mode solution (SOL 103) with NX NASTRAN, and in an optional dynamic response calculation (SOLs 111 and 112). In the normal mode solution, contact stiffness result is added from the end of the converged linear statics contact solution. The contact stiffness values in the normal mode solution represents the final contact condition of the structure around the contact interface. Thus, it will appear that the resulting contact edges or surfaces are attached during the normal mode analysis. Since the calculated normal modes include the final contact interface conditions, the response calculation (SOLs 111 and 112) which use these normal modes automatically include the same conditions.
The inputs for the normal mode solution are consistent with differential stiffness solutions which require a linear statics subcase. The difference is that the linear statics subcase should include the BCSET case control command. When defining the normal modes subcase, a
STATSUB case control command must be included to reference the subcase id containing the contact definition. The contact solution in the linear statics subcase must fully converge before moving to the normal mode portion of the run.
Contact conditions can be used with the element iterative solver. However, differential stiffness conditions cannot be generated with the element iterative solver. Therefore, the default sparse solver will always be used, even when the element iterative solver is requested.
Take a look to this post:
Best regards,
Blsa.
~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director
IBERISA
48011 BILBAO (SPAIN)
WEB:
Blog de FEMAP & NX Nastran:
