Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

No convergence with GAP element

Dear all,

 

I need an help with a non linear analysis.

I have a model with gap element that modelling contact between shell elements.

First of all, I perform a linear elastic analysis with "gap as contact" option, follow the indication reported on a post of @Blas_Molero.

This first analysis is done without any problem (I also read the .f06 file to be sure that non errors are generated).

Then I would like to perform a NL analysis with the same model, but at the first iteration I obtain a convergence problem..

 

NL.PNGNL setting

 

Please could anyone help me? 

 

Best regards

Stefano

5 REPLIES

Re: No convergence with GAP element

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

Search the *.f06 file for FATAL and post the error message content here.

Best regards,
Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: No convergence with GAP element

Dear Blas,

 

I attach at this post the .f06 file and the fatal error message.

 

*** USER FATAL MESSAGE 4551 (NCONVG)
*** STOPPED PROBLEM DUE TO FAILED CONVERGENCE
User information:
A solution is not possible. Review NLPARM requests and modify
to select a better solution approach.

 

Best regards

Stefano

Re: No convergence with GAP element

Genius
Genius

I did a lot of non-linear analyzes with simulated contacts through gap elements, but every time I had to use mesh with hexaedric elements otherwise I did not get convergence.

 

P.S. I never understood why. The Basic Nonlinear Analysis User's Guide at point 1.7 suggests to avoid CTRIA3 and CTETRA, and I suggest you to read it carefully. Finally I always increase the standard tollerance to reduce the computing time, but this may be due to my computer...

 

Best Regards

AMinati

Re: No convergence with GAP element

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Hello!,

If the linear static contact analysis (SOL101) runs OK and the nonlinear (SOL106) fails surelly either you have a rigid body motion or you have reached an stability bifurgation point (nonlinear buckling), without the model in hand is difficult to know the exact reason. Please note in linear static analysis you have "PARAM,AUTOSPC,YES" keyword activated by default, but in SOL106 this is useless. Also I see revising the *.F06 that your mesh is not good, you have many violations of NX NASTRAN mesh quality check and in nonlinear analysis the element quality is critical, bad mesh quality can cause the solution diverge.

Best regards,
Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: No convergence with GAP element

Dear @Blas_Molero,

 

there was a problem of rigid body motion in my model. The gap elements will activated only after an adequate preload...

I've checked mesh quality by mean of NX nastran Criteria, but the distorted elements are positioned in a low stress gradient region and are 94 of 150k... 

I also try with a simplified model, in order to replicate @AMinati problem, but I don't obtain particular problem.

@AMinati, if you want to talk more about this problem, please send me a private mail.

 

Best regards and tanks!

 

Eng. Stefano Milani