How to include global contact parameters during Normal modal analysis in NX Nastran 7.5 2

[Jai460]

I want to perform modal analysis for a component by considering contact parameter with other component.I am using NX NASTRAN Solver.Solution type: SEMODES 103.I have included contact parameters(Source region and Target Region) in the deck.But i am getting results in such a way that contact region is not at all considered in the modal analysis.So please guide me.I would like to know how to include contact parameters in the modal analysis.
The main aim of this project is to find out the contact force extracted by target component on the source component during Modal Analysis.
Thanks in Advance.

 

[BlasMolero]

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:

https://iberisa.wordpress.com/2011/...-ensamblaje-con-contactos-surface-to-surface/

Best regards,
Blsa.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[GregLocock]

However, from a practical standpoint, assuming contacts are engaged during a modal does not represent typical cases found in assemblies.

There is no simple solution to this, various methods are employed to linearise the system in a real test. These include, excitation using a sine sweep at one amplitude, excitation using gaussian white noise and taking an average, hot glueing all intermittent contacts together, removing rattling components.



Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?