UGNX Nastran Non Linear Contact

[thecadguy]

Dear All,

I need some help using non linear contact simulating a pinch joint. I am using sol 601,106 with the main part contrained in 1-6. A load is being applied to the ears of this part that clamp around a stud that is inserted thur an opening in the main part. There is an initial gap of .1mm.

I think the problem is rigid body motion in the stud so I added weak springs to help stabilized until the first convergence. I use the ATS and MSTAB options to also help.

Most times the model does not converge but when it does, the main part still penetrate thur the stud and there is no stress on the stud.

As soon as I placed a rigid contraint on a couple nodes it works fine and clamps around the stud and produces stress and strains. this tells me that the springs are not doing what they were supposed to even though I have tried various stiffness values.

Can anyone provide any other recommendations so that I may get this to work without adding these fixed constraint which adds artifical stresses in the model.

Is there any other options that need to be turned on. The main part is alum and the stud is steel.

Thanks

 

[BlasMolero]

Hello!,
If any part is free to move, then first task will be to stabilize that component in order to avoid rigid body movements, you can use soft springs, or activate contact friction, or use CGAP node-to-node contact elements.

The "general" basic advices for nonlinear contact are the following:
• Add or remove friction.
• Use small displacement contact instead of large displacement contact (CTDISP)
• Add contact compliance (CFACTOR1)
• Increase friction regularization parameter (EPST)
• Gradually remove initial penetrations (INIPENE/TZPENE)

To improve conditining do the following:
• Add boundary conditions (restraints)
• Add supporting springs
• Add stiffness stabilization (MSTAB/MSFAC)
• Use prescribed displacements instead of forces where possible
• Add contact damping (CTDAMP)
• Limit maximum displacements (MAXDISP)

In case of divergence of contact solution (or slowly converging), even with ATS, the "basic" recomendations are the following:
• Allow more iterations (MAXITE)
• Use deformation independent loads (LOADOPT)
• Use smaller time steps (TSTEP)
• Toggle line search (LSEARCH)

In NX NASTRAN Advanced Simulation (SOL601) we have much more resources to help contact convergence, but without yhe model in hand is dificult to tell you what happens in your model, sometimes basic items like mesh quality & density are critical to get success in nonlinear contact analysis, OK?.
Good luck!!.
Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[thecadguy]

THANKS I THINK I MAY HAVE IT WORKING. ONE QUESTION IT APPEARS SOL 601 DOES NOT HAVE SUBCASES. HOW WOULD YOU CALCULATE THE PIN PULLOUT FORCE ONCE THE CONTACT CLAMP PRESSURE HAS BEEN APPLIED AFTER THE SOLUTION. I CAN POST PROCESS THE CONTACT FORCE AND ?PRESSURE BUT AM NOT SURE HOW THIS RELATES TO PULL ?OUT FORCE. WOULD I NEED ANOTHER TIME STEP SOLUTION.?

 

[BlasMolero]

Hello!,
The key is to use RESTART, or to use ARRIVAL TIME using time functions to apply, for instance, displacements at a later time to a deforming configuration resulting from the applied load.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[thecadguy]

Dear Blas,

Thanks for the tip, I understand the concept and am still new to NX. so would you recommend the arrival time instead of the restart? Would you recommend an enforced displacement of the pin to start right after the clamp load time has finished? If so, would you do the entire length of the pin or a percentage of the pin length? What would I have to evalaute in the post process to actually calcuate the pull out force to break the clamp pressure and static friction?

Again, thanks for your help.

THECAD GUY

 

[BlasMolero]

Hello!,
Uff, too many questions, whitout the model in hand is very difficult to tell you the best strategy, but the foundation in NX NASTRAN Advancd Nonlinear to manage "process" is using function time curves to control activation of loads & prescribed displacements. Aditionaly you have RESTART feature.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[thecadguy]

Dear Blas,

thanks sorry to over load you. I have tried to time funciton the loads with tables. However, one last question. Do you recommend single intervals or multiple intervals on the time steps. I have the first load ending at 1s and the second load starting at 1s and going to 2s. I get an error message stating the times are not aligned? Should I cram it all in one single interval or keep with the multiple but maybe need some overlap?

ANy thoughts

 

[BlasMolero]

Hello!,
All time curves must spand the same interval, it not error. If a time curve is not longer active, the function should be zero, but span till the end of the analysis, OK?.
Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Boghya]

Dear Blas,

Quite some usefull info about the contact problem.
I would have a question about contact in transient analysis...
So for the begining...
the problem...2 rows of solid elements placed at a certain distance one from each other, the ends are fixed and on one of them there is a pressure applied
the setup...there is contact between the 2 rows, 2 analysis are setup (for the same model..mesh...contact setup...): static and transient. Transient has time 5sec all the loads are from t=0 to t=5 constant value
the results...static analysis runs with no problem..transient on the other hand doesen't want to run (the problem seems to be the negative Jacobian that ADINA is obtaining)

The time step increment is set to AUTO...so he tries to make smaller time steps...but everytime he is obtaining negative Jacobian...even thou the mesh is quite refined

Any suggestion?

 

[BlasMolero]

Hello!,
If diverging solution then stabilize the model with stiffness stabilization, contact damping or low speed dynamics.
Also reduce convergence tolerances and add slight damping in Newmark.
Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/