Mesh size Radioss crash simulation

Philipp Link
Philipp Link Altair Community Member
edited November 2020 in Community Q&A

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

Tagged:

Answers

  • ArthurJANNOT
    ArthurJANNOT
    Altair Employee
    edited November 2020

    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
    Juan_Pedro_Berro
    Altair Employee
    edited November 2020

    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
    Philipp Link Altair Community Member
    edited November 2020

    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

     

  • ArthurJANNOT
    ArthurJANNOT
    Altair Employee
    edited November 2020
    Philipp Link said:

    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

  • Philipp Link
    Philipp Link Altair Community Member
    edited November 2020
    Arthur JANNOT_20986 said:

    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

Categories