Modal Analysis of an Assembly

[generaluday]

Hello,

I've been trying to conduct a Modal Analysis of a simple assembly (the example assembly provided in the help system) in FEMAP. I tried this on a lamp assembly of my own, and since it didn't work the way I'd anticipated, I thought I'd try it on a simpler assembly first.

I just deleted the load on the front surface of the "plunger" and ran a modal analysis, but I'm obtaining similar results as I did with the lamp, in that the mode shapes comprise of the individual components becoming dis-engaged and vibrating irrespective of the assembly "contact" constraints.

How do I fix this? How do I have the mode shapes account for the assembly constraints, i.e., have the plunger not disengage from the base link which are connected using the pin which slides through the holes in the former components?

Thanks.

 

[generaluday]

Also, I read the "Linear Contact in Normal Modes analysis," and, according to namklof's suggestion, changed the "contact" condition to "glued," but that did not work either. The solver just failed.

It makes perfect sense that a "contact" problem would call for a non-linear solution, and that the "normal modes" analysis requires a linear model.

Does anyone have any ideas as to how to obtain the normal modes of an assembly while maintaining the contact constraints between the components of an assembly?

 

[francesco87]

Linear contact in a Normal Modes Analysis requires a pre-stiffened analysis as a subcas: the solver needs to add the differential stiffness coming from the contact conditions, in order to account for the contact constraints.

I copy here the paragraph "Special Note about Pre-Stiffened Modal Analysis", page 8-69 on the FEMAP User's Guide:

"You will notice that during a Normal Modes analysis, that you cannot choose a Load Set in the Boundary Conditions
dialog box of the Master Analysis Case. You can run a pre-stiffened modal analysis in FEMAP by adding a
loading condition to your model, but it does require a subcase to be created in order for it to work properly. The
exact process is to go to the bottom of the “tree structure” in the Analysis Set Manager and highlight the “No Case
Defined” branch of the “tree”. Now click the New button and FEMAP will prompt you to create a subcase. Click
Next and you can now add a loading condition to the model using the Loads pull-down menu (you will need to have
a load set for this to work properly). You will notice an additional SUBCASE has been added to the Case Control
section and a STATSUB entry can be found there which will prompt Nastran to run a Pre-stiffened Modal Analysis.
Now run the analysis and your results will reflect pre-stiffened modal analysis. A pre-stiffened modal analysis is
needed when using Linear Contact with NX Nastran SOL 103."