Mesh size Radioss crash simulation

Hello!

I have created two identical simulation models for a crash beam.

The only difference between both models is the mesh size: 4mm quads on the one hand and 2mm quads on the other. Unfortunatly, the model with the 2mm quads mesh shows unexpected physical behauviour, while the other one looks fine.

I have read about the recommondation to use mesh size >= 5mm, but how does the mesh size influence the simulation and what problems accour with small mesh sizes?

Thank you for your help

Find more posts tagged with

English

HyperMesh

Radioss

v2019.1

Accepted answers

All comments

ArthurJANNOT

Hello,

The mesh has a different influence in your calculation, in the event of crash you have for example dependence of the time step.
The finer your mesh, the smaller the time step. If you have the same time step for your both simulations, Radioss will use added mass to balance in case of your small mesh.
You must pay attention to your contact and the ratio of thickness to your mesh.

It's possible to share your twp models to understand what are "unexpected physical behauviour" please?
Regards
Arthur

Juan_Pedro_Berro

Hi,

Pay attention to contact and gap value vs mesh size. It can produce unphysical behavior from cycle 0. Can you describe a little bit more your model/behavior?

Best regards,

Juan Pedro

Philipp Link

Hello,

thanks for the fast response!

Please find attached my two models. Does the Gapmin value always need to be half of the thinnest part?

Best Regards,

Philipp

CSE13-0101_Beam_S355.hm

CSE13-0102_Beam_S355.hm

ArthurJANNOT

Hello,

thanks for the fast response!

Please find attached my two models. Does the Gapmin value always need to be half of the thinnest part?

Best Regards,

Philipp

Hello,

Thanks for your model.
The problem on your model is that the gap calculated is 2.52mm (sum of half thickness 2.52/2 + 2.52/2 = 2.52 that is higher than your element size). The consequence is that every node are already penetrated.
To avoid that, you can use parameters : Irem_gap = 2, adapt %mesh-size when using Igap = 3, and Iadm = 2.
To have more details on those parameters, you can have a look of online help about /TYPE7 interface.
You will find attached the model that I have modified.

Due to the thickness of 2.52mm and mesh size of 2mm, you are in the limitation of shell theory.
If you need to refine the mesh, I suggest you to use thick shell or volume.

Does it answer to your question?

Regards.

Arthur

COMPARE_MESH_SIZE-parameters.png

CSE13-0102_Beam_S355_correct2_0000.rad

CSE13-0102_Beam_S355_correct2_0001.rad

Philipp Link

Hello,

Thanks for your model.
The problem on your model is that the gap calculated is 2.52mm (sum of half thickness 2.52/2 + 2.52/2 = 2.52 that is higher than your element size). The consequence is that every node are already penetrated.
To avoid that, you can use parameters : Irem_gap = 2, adapt %mesh-size when using Igap = 3, and Iadm = 2.
To have more details on those parameters, you can have a look of online help about /TYPE7 interface.
You will find attached the model that I have modified.

Due to the thickness of 2.52mm and mesh size of 2mm, you are in the limitation of shell theory.
If you need to refine the mesh, I suggest you to use thick shell or volume.

Does it answer to your question?

Regards.

Arthur

Thanks a lot!

That really helped me to understand the problem.

Best Regards,

Philipp