No Penetration SOL103 1

[DOFxyz]

Hello everybody...

Is there a way to use SOL103 to model two (2) panels that are either Spot-Welded or Bolt-Jointed.

I have used "Surface-To-Surface Glueing" at few elements but when I run the model the plates go inside each other!!!

Is there a way to tell NASTRAN "look there is a material there you can not go through it!!!"

Regards;

 

[ESPcomposites]

You can run a contact analysis with SOL600.

Short of that, you could use a gap element for a simplified representation of contact (SOL101).

Brian

http://www.espcomposites.com

 

[DOFxyz]

I've attempted to use a CGAP element but the SOL101 does not like it. I think this element is non-linear only!!!

I've tried to use "surface-to-surface contact" it seems to work, but I still have some fea elements that penetrate each other!!!

It might have to do with the settings of the "surface-to-surface contact" option, e.g. penalties, no. of active elements...etc.

Would you have a simple example that works (using CGAP)?

PS. I have dived into NX & NX-NASTRAN user manaual (not an easy task!) and they recomend using the "surface-to-surface contact" and do the solution in two steps 101 then 103. (pending that I understood the manual correctly!!!)

Regards;

 

[truckcab]

Hi,
since SOL103 is the solution sequence for the computation of real eigenvalues i.e. it is a strictly linear analysis you can, per definition, not include contacts. If you have penetrations e.g. shell meshes crossing each other you will have to solve that issue in an other manner than using contact conditions. The problem is that you can not simulate gaps meaning that any "fake" contact of yours will not be able to simulate separation. This is a limitation of SOL103 and lies within its theoretical background. If you want to simulate proper contact then SOL103 is not the solution sequence for you.

I guess youll have to use a non-linear dynamic approach to solve your problem properly.



Live Long and Prosper !

 

[DOFxyz]

truckcab

In short I think you are right.

regards;

 

[BlasMolero]

Hello!,
NX Nastran provides a contact capability for SOL 101 linear static analysis, and also in consecutive SOLs 103, 111 and 112. Contact for the SOLs 601 and 701 is also available. Contact conditions allow the solution to search and detect when element faces come into contact. The software then creates contact elements, thus preventing the faces from penetrating and allowing finite sliding with optional friction effects.

A contact condition can be included in a normal mode solution (SOL 103), 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 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 bulk entry 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.

Hope it helps!!.
Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com