THE *FAIL STRESS OPTION CAN ONLY BE USED WITH PLANE STRESS ELEMENTS? 2

[Mohcine]

I got this error in my simulation:
"THE *FAIL STRESS OPTION CAN ONLY BE USED WITH PLANE STRESS ELEMENTS"

I tried looking at the manual , but couldn't figured out how to overcome this problem.


Any suggestions?

Thanks in advance

 

[compositesFEAguru]

Hi Mohcine,

You are probably using continuum solid elements (C3D8R) with solid sections. To use the composite failure criteria in Abaqus, you must use continuum shell elements (SC8R) with shell sections.

Hope this helps

Firehole Composites

http://www.firehole.com

 

[Mohcine]

Thank you , that solved the problem.

 

[Mohcine]

When I modeled the composite as a shell, I get distortion errors and the job is aborted.
When I use 3D solid continnuum element, no distortion takes place and the jobs runs until the it is completed.

This happened as I was making the mesh finer. Any Ideas?

Thanks

 

[compositesFEAguru]

Hi Mohcine,

Are you modeling progressive damage using the Hashin failure criterion? Do you have nonlinear geometry turned on (NLGEOM=YES) in *STEP card? Both of these things could be causing element distortion errors. You may not be seeing it for 3D solids because you are not modeling damage...?

Regards,

Firehole Composites

http://www.firehole.com

 

[Mohcine]

Yes am eventually modelling progressive damage...But for now , I removed the damage parameter from the composite material and the cohesive interaction t speed up the simulation i'm carrying out mesh study. When I use solid element , no errors encountered, however, when I use shell element (which seems to allow the usage of fail stress) error occurs and results in the job being aborted (for very fine mesh) :

Excessive incremental rotation of the elements in element set ErrElemExcessIncrementalRotation-Step1.

There is only one element with excessive rotations


The NLGEOM is always on . I have included a picture of the last frame before the analysis is aborted.

My wild guess is that as the mesh is made finer, the contact force increases hence more distortion.

Thanks for your help

 

[compositesFEAguru]

Didn't know you were using Explicit. Sorry but I am unfamiliar with Explicit and the errors associated with it.

Firehole Composites

http://www.firehole.com

 

[Mohcine]

I see ...many thanks for your commendable intention to help me . Words can not express my gratitude.

I love your blog by the way, It has something informative, easy to follow posts.

 

[IceBreakerSours]

I am not sure if this is going to be any help but here are my two cents:

Node on structural elements such as shell elements not only have translational but also rotational degrees of freedom. If you do not restrain DOFs appropriately, you'll end up encountering unexpected issues.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Mohcine]

I applied encastre boundary conditions at all the four edges...But I will change the those conditions and see if that helps. Thanks for the suggestion . I might also try using kinematic instead of penalty for the contact constrain and see if it helps.

Thanks again

 

[IceBreakerSours]

Encastre restrains *all* DOFs. So, you are preventing all edges from rotating OR translating. I am not sure (since I don't know the geometry/mesh in your model) but you might want to look at rotational DOFs of the nodes inside the domain.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[IceBreakerSours]

I must qualify my previous statements. This DOF business that I've been going on about is applicable only to conventional shells and not continuum shells. Nodes on continuum shells have translational DOFs only. If you have not, try to use conventional shells for your analysis (but make sure thickness change is "small"; see "Stress/displacement continuum shell elements" in the Analysis User's Manual for details.) They are more suitable for nonlinear geometric analysis. However, I recommend going through the "Choosing a shell element" section of the Analysis User's Manual before you start experimenting.

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Mohcine]

That sounds like a good idea..I will try it and report back when I have. Is there an easy way to convert a contiuum shell to conventional shell? As i did for solid to shell?

Apologies for the late reply, my laptop broke and i had no means of replying.

 

[Mohcine]

I have used conventional shell (2D) and didn't encounter any problem as I previously did.

I have wanted to make that clear, just in case some else in future experiences similar error.

 

[Mohcine]

@compositesFEAguru I would like to get in contact please . I wish to mention you in my acknowledgement, for helping me alot.
Thanks

 

[compositesFEAguru]

@Mohcine - You can connect with me on LinkedIn by clicking on the link on the right side of our blog (

http://info.firehole.com/blog).

You are most welcome!

Firehole Composites

http://www.firehole.com