applied load vs breaking load, non-linear static (SOL 106) 1

[tstanley]

Hi:

I have used linear static analysis for many years but have recently switched from NEiNastran to NX Nastran which gives me the ability to do non-linear static.

My test model is of a four bar test on a composite panel. The foam core is non-linear solid elements with skins of laminate shell elements. For the foam material a function was entered with the approximate stress strain curve based on actual tests. The material properties seemed to work well on a smaller simpler model. With the four bar test a couple of runs generated fatal memory messages so I increased the database memory in the preferences, still in the "yellow" range. Following that the analysis seemed to be going OK from looking at the f06 file. All iterations were converging up to loopid 35 (23 hours or so). After that for an additional 10 hours, no more iterations were run, it stayed at loopid 35 with a load step value of 0.74 .

This is a long winded preamble to my question. What happens when the load applied in the case makes the material exceed the strain indicated in the function graph, which ends where the material breaks? I would expect a warning message or a fatal error, but none of these were generated.

Any help would be appreciated.

Tom

 

[BlasMolero]

Dear Tom,
First at all let me tell you that the RAM memory should not be increased in the FEMAP preferences, no, this setting is for FEMAP only (the pre&postprocessor), please let the dafault value as before (in the green range). You need to assign more RAM memory for the NX NASTRAN solver, not to FEMAP, ok?. This is done during the analysis study definition in the NASTRAN Executive & Solution options: by default you have mem=estimate, then try a value of say 5GB, write 5*1024 and see if the problem progress. If required use 6*1024

Regarding your question, I don't know exactly what will be (the test is easy, make a little model and define a load that generate strains above the value defined in the material stress-strain curve), but I can tell you that the basic NX Nastran Nonlinear (SOL106) solver is generally limited to strain rates less than say 10-15%, then surely you will reach this limit in cases of large strain problems. The theory implemented in NX Nastran is adequate only for small strains (less than 20%) in multiaxial stress state as it is not based on the classical theory of finite elasticity. For large strains in multiaxial state, you should use a hyperelastic material instead.

Best regards,
Blas.

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

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[tstanley]

Thank you Blas:

My old NEi had something similar that I had forgotten about. Thanks for the tip on where to find the setting. I tried it at 6*1024 but still ran out of memory. Then I discovered that my virtual memory setting in Windows was set lower than I expected. I will try again.

Regarding the change to hyperelastic material, I am reluctant to try it because of lack of knowledge about the hyperelastic properties. However my material does seem to work OK on my smaller model. The maximum strain that was used is 0.25. The small model ends with a non-convergence message. When the results are recovered, the maximum non-linear shear result is 0.248 which corresponds pretty well and it makes sense that it wouldn't converge at that point.

Tom

 

[tstanley]

No Luck.

With increased memory it again stops doing anything at the same loopid as when it ran out of memory. Status is active but no further action or messages. Pressed kill job and got acknowledgement in Femap message area, but Nastran continues "not responding". "end task" doesn't work. Had to manually turn off the computer with the power button.

Time for tech support I think. Also learn about hyperelastic material.

Tom

 

[BlasMolero]

Dear Tom,
If the computer gets locked, then you need to increase your RAM memory to solve the I/O problem botlneck generated by the scratch data.
Take a look to this material, is critical to correctly Windows turnning for NX NASTRAN:

http://community.plm.automation.sie...XNastran_forum/22/1/windows_perf_tuning_1.pdf

Best regards,
Blas.

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

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[tstanley]

Thanks Blas:

I read the info you linked to and it was useful. I not only disconnected from the internet and turned everything else off, but also disabled my virus checker as it suggested. This all helped with the speed. I still have memory issues though. There seems to be a file size limit, not so much a limit of hard drive space or virtual memory space.

It solved and gave results on my last test although it took a couple of hours to get the results after the analysis was completed. I could see it still working through the f04 file. The final change that allowed it to complete was to reduce the load so that the maximum strain was just below the maximum strain allowed on my function graph. I was told though that when the calculations come to the end of the graph it just assumes that the graph continues on at the same slope. So I can't say for sure that having the strain exceed the allowable (on the graph) was the answer to my problem. It will take more trials to find that out.

Tom