ARAMID/EPOXY (ZERO DEFORMATION) PROBLEM 1

[Oluwakay]

Good morning Ladies and Gentlemen. I hope you are fine. I've been struggling with ballistic impact on aramid/epoxy composite. I used J-C damage model for the bullet and Hashin damage model for the composite. When I tried to run the job, the composite stays rigid and undeformed, whereas the does just as we had it from the experiment. Perhaps I modelled the composite wrongly, this I am not sure. I would appreciate every help I can get. This work is giving me tough time and its choking me. I'd also appreciate if you'd like to look into the file for me and point out some possible mistakes I might have made
Thank you all!

 

[FEA way]

Are damage and STATUS variables requested for field output and is element deletion enabled ? Is contact defined properly and does it detect the interactions between the parts ? Which type of elements are you using ? If you can share the .inp file, it will be easier to help.

 

[Oluwakay]

Thank you so much for your feedback. I have attached the .INP file to this reply.
Thanks a lot, I really appreciate it.

 

[FEA way]

Try changing the stack direction of continuum shell elements - it should be oriented between the top and the bottom of the plate.

 

[Oluwakay]

Thank you for your response. However, I am so sorry I do not understand what you are trying to explain. Could you shed more light please? Thank you once again.

 

[FEA way]

In the Mesh module open the plate part. Use Query —> Mesh stack orientation to see how the mesh stack direction is currently assigned. It should be changed so that the brown and purple colored faces are the top and bottom, not the side ones. Use the Assign Stack Direction tool to change this.

 

[Oluwakay]

Thank you once again. I have done what you said and I got this feedback: 12150 elements have missing property definitions. The elements have been identified in element set ErrElemMissingSection.
Analysis Input File Processor exited with an error.

I have attached the updated INP file to this response and the new job is titled "test_8"
I really appreciate your time and effort.
Best regards.

 

[Oluwakay]

I just attached it. Thanks

 

[FEA way]

Make sure that the section/composite layup and element types match each other. For example, if a composite layup is defined for conventional shell elements, those elements have to be used for this part.

 

[Oluwakay]

Thank you again for your feedback. I tried to correct what you pointed out, ran it, but no single deformation appeared on the composite plate. Only the projectile deformed. I really appreciate your effort so far. I have attached the updated file to this feedback.
Best regards.

 

[FEA way]

Can you share the .cae file as well ? It will be easier to do some tests, especially involving mesh modifications. To find the source of the problem you can try removing and replacing features in the model. For example, try with conventional shell elements instead of continuum shells.

 

[Oluwakay]

Good morning. I am sorry it took a while before I returned a feedback. I was out of town. Fortunately, it has worked out. Thank you so much, you are such a great help.

 

[FEA way]

Great that it's working now. Can you say what was causing the problem and how you fixed it ?

 

[Oluwakay]

Yes.
Under the section of field output, no parameters connected to hashin damage were checked. I had to check them all and ran it again and lo and behold, it worked!
Thank you so much, you really helped me.