NLSTAT or NLGEOM

Altair Forum User

Hello,

I want to know for doing a non linear analysis whether we can use the NLSTAT option or not. I have a plastic component so I have to perform a non linear analysis. Which option should I use?

Rahul Rajan_21763

Hi,

Please use analysis type as NLSTAT.Use MAT1 with MATS1 card for defining nonlinear material.For Detailed information please go through Optistrcut user guide.

Regards

Rahul R

Altair Forum User

If I use NLSTAT, the error is 

 

*** ERROR # 4068 ***

 TYPE = 'NLELAST' is only supported in NLGEOM, IMPDYN and EXPDYN subcases.

 

And if I use NLGEOM, the results eg. stress is coming as zero. 

 

I have used MAT1 with MATS1 card. I am following the user guide but still I am not able to get the results.

Altair Forum User

Hi Priyanka,

 

what is the material you are using?

 

is it non-linear elastic material (ex: rubber, foam, etc..) ?

 

If not, please change the TYPE in MATS1 card to PLASTIC instead of NELAST.

Altair Forum User

Hi,

 

Yes it worked. Thank you so much.

Altair Forum User

Hello,

 

you have to know, that NLSTAT only supports small displacements AND small strains.

Typically NLSTAT is used for GAP analysis or nonlinear material with very small strains.

 

For NLGEOM and shells, Hyperworks is using the implicit module of Radioss. The deck, analysis and results are differ from Optistruct.

 

Best Regards,

Mario

Altair Forum User

Adding to the above Large displacement analysis, where large strains are involved can be possible with Large Displacement  Non-linear static analysis.

 

This feature is available from HW 13.0 and only supports SOLID ELEMENTS.

Subhu_21017

Hi Prakash,

 

Is it possible to do a NLGEOM analysis for 1D elements with nonlinear material property?

Or the NLGEOM only for shell and solid..?

Altair Forum User

Hi Subhu,

 

MATS1, which takes the non linear material data is not supported for 1D elements. But you can use 1D elements in NLGEOM.

Altair Forum User

Hi,

 

I have a problem about s-s curve. S-S Curve starts 0.0 and 0.0. So, I selected TYPE is NLELAST. But I cant run as nonlinear quasi-static. I changed S-S curve values, that is,Strain point is 0.0, stress (yield stress) is 48. and LIMIT1 is 48. Type is Plastic. I run it again. the error is

 

  (this is continuation line 1 of TABLES1,13 bulk data)
  '+            0.0    48.0    0.02   48.14    0.02   48.42    0.02   48.68'
 
 *** ERROR # 1127 *** in the input data:
 Discontinuities are not allowed at TABLES1 endpoints.

 

What should I do for this problem?

 

Thanks

Altair Forum User

Hi Nihan,

 

Maybe this picture from OptiStruct help can give you some idea /emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20'> 

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

Hi Prakash,

 

Woow!! I got it. Thank you. /emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' />