Non-linear buckling analysis in ANSYS

[rh142]

ANSYS help recomends that if SSTIFF is used for non-linear buckling analysis adaptive decent should be turned off to get a lower bound. What if SSTIFF is turned off?

I have found that adaptive descent is helpfull when doing elastic-plastic analysis, turning it off will give an unrealistic low number.

Any insight is welcome.

Thanks,

 

[yugabalan]

Hi rh142,

I am not sure where you got the information from. However, I'd assume you are refering to non-linear analysis without and upgeom consideration. If so, then this is not a buckling problem at all.

Typically in non-linear buckling analysis, an initial linear static analysis is carried out with pstres,on. This is to obtain the stress stiffness matrix that would be used in the second stage of analysis, the eigenbuckling analysis analysis.

Ansys recommends either one option to be used, pstres or sstif option. Note that sstif is an option only when nlgeom,on. In other words, the eigen solution, which is linear static based is totally impossible with the sstif option.

I could assist you if you're able to give me a clearer picture on what you are working on.

YGK

 

[rh142]

YGK,

Thanks for the response. I am looking under ANSYS help section 7.3 Performing a Nonlinear buckling analysis of ANSYS10 help. Specfically in section 7.3.2 for automatic time stepping.

I am trying to calculate the buckling of a flexible composite plate structure. I need to take into account plastic behavior, contacts, gaps, and large-deflection response. Which is why I am using the nonlinear buckling analysis instead of the eigenvalue approach. From what I understand nonlinear buckling analysis approach is just static analysis with loads increasing untill the structure buckles.

Thanks,

 

[Yoman228]

How good are they in Ansys in doing the Nonlinear buckling analysis compared to ABAQUS?

 

[yugabalan]

rh 142,

I think you have very crude understanding of non-linear buckling analysis. But its ok. I will try my best to explain it to you.

One good thing about Ansys is its help documentation, where you can get very good information. I would strong recommend you to read through 'how to perform non-linear buckling analysis'. Dont mix up non-linear static analysis with non-linear buckling analysis. As i've mentioned to you in my earlier reply, non-linear buckling analysis takes into consideration structural imperfection magnitude (upgeom).

Structural imperfection magnitude can be obtained in many reference standards or rules or handbook. and this should correspond to the 'imperfect' shape or the eigenmodes you would obtain from the eigen buckling analysis. And as you can see, you have to perform an eigenbuckling analysis to determine the eigenmodes, else its tricky to determine the structural mode responses.

Simplified, you MUST to do ALL the followings: (a) perform linear static analysis with pstres,on (b) perform eigenbuckling analysis (c) determine which mode shape you wanted to use in the non-linear analysis, typically the 1st mode will be crucial (d) determine the imperfection magnitude from any reference (i always refer to DNV OS C 401, as fabrication tolerance) (e) impose non-linear material model, geometry, apply imperfection on the eigen mode you choose and solve using progressive load increments (f) your ultimate buckling load corresponds to your last converged substep.

Hope this helps!


Yoman228,
The FE solver source codes are more or less the same. So the results will be almost identical. The difference is on the pre-post facilities you have in a FE program.

Explicit codes like ls dyna gives better dynamic result if you are trying to investigate buckling load problem beyond the snap thru point. Good luck to you.

Yugabalan K

 

[rh142]

Yugabalan,

Thanks for the input, I agree that initial imperfections also need to be taken into account. My question is relating to steps e and f. When calculating the ultimate buckling load the switches in the program do make a difference where you final converged load step is. If I turn adaptive descent on or off.

R

 

[yugabalan]

I am assuming here that 'adaptive descent' means automatic time steping. Is this what you are refering to?

If so, it is obvious that with the automatic time stepping you will end up with better result, but longer in solving time. It is also important to know that your time step size will also effect the accuracy of your result.

Without automatic time stepping, each steps are equal in in 'size'. Bisection of of steps will not take place either. You could end up in lower buckling load, but conservative. Then again, its all depends on you whether you want a fast analysis or an accurate one. Cheers!

-Yugabalan K