Linear Contact in Normal Modes analysis

[francesco87]

Hi everybody, this is my first thread.
I'm a beginner with Femap and Nastran, therefore there could be some basics I ignore or I'm not familiar with: I would be very grateful if you gave me some general tips, besides the specific issue in subject.

I'm using Femap v.10.2 with NX Nastran to analyse a PCB assembly (please find attached a picture).
My model consists of a PCB, a chip, some plastic connectors and an aluminium frame, all connected via bolted joints; I modeled everything with solid elements (tetra). I simulated the joints by means of spider curves at the top and the bottom of each hole, connecting their center by a RBE2 element, and I used the "Connect - Automatic" command to detect contacts between surfaces.

Everything seems to work fine but when I run the Normal Modes analysis and animate the modes, all the parts being in contact penetrate each other, whereas with the Linear Static analysis every contact is worked out correctly.

Thanks in advance.

 

[namklof]

If you did define contact surfaces, the linear static solution requires an iterative solution process (and technically is a nonlinear solution). A normal modes analysis requires a linear model. I believe if contact surfaces are present, the use a default setting which is probably no contact and this setting is maintained. Thus you have parts moving through one another. To complete a normal modes analysis, you might consider changing from contact surface to glued surfaces (under connection properties). Depending on your problem, this may give reasonable results.

 

[BlasMolero]

Dear Francesco87,
With FEMAP & NX NASTRAN you can use "Linear contact in a Normal Modes solution (SOL103)", the ability to define beam elements as preloaded bolts, and the ability to include the contact stiffness from a converged surface to surface contact solution in a normal mode solution (SOL 103) is available en NX NASTRAN since version V5.0 (April 2007).

In the normal mode solution, NX Nastran adds the differential stiffness calculated from the bolt preload analysis, and the contact stiffness resulting from the converged linear static contact solution to the structural stiffness. The contact stiffness values in the normal mode solution represent the final contact condition of the structure around the contact interface. Thus, it will appear that the resulting contact surfaces are attached during the normal mode analysis.

The inputs for the normal mode solution are consistent with differential stiffness solutions which require a linear static subcase. The difference is that the linear static subcase should include the BCSET case control command. When defining the normal modes subcase, a STATSUB bulk entry must be included to reference the subcase id containing the contact definition. The contact solution in the linear static subcase must fully converge before moving to the normal mode portion of the run.

Note that since the calculated normal modes include the final contact interface conditions, the modal response solutions (SOLs 111 and 112) which use these normal modes automatically include the same conditions, then you see here a window for considering contact in advanced dynamics as well.

I hope to be able to write a tutorial in the following weeks explaining the steps to follow in FEMAP & NX NASTRAN to solve with success a modal contact problem.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

 

[francesco87]

Dear Blas,
thank you very much for your detailed and clear explanation. Besides, I've seen many of your tutorials and they're extremely helpful and well done.

I'll follow your tips and check your website in the next weeks.

Regards,
Francesco