Contact failure

protontimprotontim
I have a model utilizing the non-linear contact of CCX that I created and ran in V20, and it worked just fine. I upgraded to V23 (and hastily removed V20) and created a similar model, but that model does not run. It starts out with exceptionally high forces and displacements and does not converge. The model created in V20 still runs fine in V23. When I recreate the exact same model in V23 however it does not work. There seems to be a problem in creating the contact - the interface is different but I have entered the same data as far as I can tell.

Two questions:

1) Where can I download V20?
2) What might be causing this failure to converge. I have exceptionally high forces and displacements at the start that do not resolve. In V20 the initial forces and displacements are reasonable and it converges quickly.

Here is a bit more info about what I am simulating.

I have a fixed mandrel that a curved bar is being bent around

The contact surfaces are between the two parts. I have modeled this with a much higher element count but show a low count here and attached.

Comments

  • VictorVictor
    Version 20 is here https://mecway.com/download/oldversions/mecway200.msi

    However, some concerns:

    The bar has no constraints against rigid body motion. That's a common reason for contact failure. I tried constraining it in Y and Z but it ended up with excessive displacement in X.

    The applied force is quite high - 18 GPa over 0.0001 m^2 is 2 MN. Is that correct?
  • protontimprotontim
    Hi Victor,

    Thank you for the link.

    1) The bar in the model is already constrained in Z and Y with the nodal constraints shown below.
    2) 18GPa is a typo that was not present in my previous more complex simulation attempts. It should be 18MPa, but it fails in either case.



    I recreated the model in V20 with 18MPa of pressure and got the same excessive X displacement. Not sure how to proceed. Seems so simple, but something is clearly wrong.

    Tim
  • protontimprotontim
    Apparently the nodal constraints are not sufficient for some reason. Using symmetry I reduced the model to 1/4 of the part and used frictionless supports for constraints, and it ran fine in V20, and I assume it will run find in V23 as well.


  • disladisla

    Strange it worked before.
    This is like a press and typically works better solved imposing displacement.
  • protontimprotontim
    edited January 10
    In this case what I am looking for is the pressure distribution at the contact surface when a screw is tightened to a specific torque. So I don't think a displacement would work. If you can make it work that way let me know.

  • JohnMJohnM
    edited January 10
    I changed your model to quasi-static and ramped the 18MPa load.
    I cheated by putting some "rubber bands" (elastic support) on the nut plate to keep things from flying away in the first steps. This is a good trick so long as you remember to use Solution->Sum to sum forces on Elastic Support Faces to be sure they are negligible.
    I recommend you try modeling solid bolts and use the pre-tension section feature, it is easy to use.

    run in v22 PASTIX

    EDIT- added bolt example
  • protontimprotontim
    John,

    Thank you for the example that was very helpful! I was unaware of the pre-tension feature and the elastic coupling trick will come in handy. Thank you again for your help.

    Tim
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register