Help apreciated

HengreHengre
Hello forum

i would appreciate if someone would have some time to look at the models attached in the ZIP-file. I am a bit confused. I tried to calculate two models. The Füll_ST_mod is the initial case. Füll_ST_mod2 has additional material to reduce y-deflection.

Unfortunately the second Model shows higher displacment ??

I used bonded contact. Are ther any Ideas?
Thanks

Comments

  • VictorVictor
    _mod2 has two copies of the force.
  • HengreHengre
    Oh my god, i was so focused on the bonded contacts that i did not see the wood for the trees,
    Many Thank's
  • VictorVictor
    No worries. There's a lot of things that can go wrong.
  • HengreHengre
    edited November 2020
    Hello,

    today I observed some interesting behaviour. (using CCX)
    I had build a model consisting of some individual parts with diferent materials. Most of then are coupled by bonded contact. between 2 there is a real contact.
    The model was meshed without showing bad elements (after some modification) and could be solved showingg reasonable results. So far so good.

    In the next step I put 2 more parts (simple cylinders of different material). Meshing was done for each of the two. The two are interconected by a bonded contact and these both then are connected to the previor existing sturcture with bonded contact.

    When I solve the 2. case I get a bunch of errormessages telling about e.g.
    *ERROR in e_c3d: nonpositive jacobian determinant in element 97 ...

    I am very confused, because all of these errors are related in the part already generated in the 1. step. No remeshing was done for them.

    Does anyony can give a exlanation for that. How can I proceed without recreating the whole model...?


    Thanks in advance

    PS: When I take the last model after aborting "Solve" and delete the additional parts of step 2 - no remeshing - the model is solved again. But the elemets indicated as bad are still there untouched ?????
  • JohnMJohnM
    The *TIE command will project nodes from the slave to master surface. This can mess up the shape of your tet10. Make sure your mating surfaces are well aligned, and use as small a number as possible for the position tolerance.
  • HengreHengre
    Thanks John,
    that I thought also, but I used 0.7 mm with the TIE command and the "problem elements" are min. 20 mm and max. 120 mm away from the last fitted bonded contacts. (?)

    I will try to do a complet remeshing with the current parameters
  • JohnMJohnM
    Check the Components section in Solution after it fails. Sometimes the solution data file has the projected geometry, and you can see what has happened. Other things to try: change the tolerance to 0.07, also try swapping surfaces.
  • HengreHengre
    I have now connected the 2 additional parts (they have bonded contact) connected to the other parts using a real contact. In this case no bad elements are shown and the model is solved,

    but still wondering about the bad elements when using bonded contact
  • VictorVictor
    I've never seen that before except the situation JohnM described where the bad elements have nodes moved by the *TIE or elastic bonded contact. Perhaps you can send me the model privately to investigate?
  • HengreHengre
    edited November 2020
    Hello Victor,

    thank you for your help. I have send you the model and some information about it.

    I hope you got the mail and you could download the file
  • HengreHengre
    Hello Victor,
    I don't want to bosther you, please let me only know if you received the model data by mail?
    Thanks
  • VictorVictor
    edited December 2020
    Oh, yes. Maybe my 3 replies were lost on the way. I'll resend from alternative account.
  • HengreHengre
    Thank you very much Victor!
    Now I got your replies by mail.
    Why it happens is still not clear to me, but you gave some valuable guidance how I could proceed.

    I had also tried some thin with *TIE to Elastic and could run the modle.

    Only it was difficult for me to really understand what are the differences in using it and how they affect the result

    Regards
  • HengreHengre
    Today I tried to do a calculation in which a round pipe is brought into a rectangular shape at one end.
    The tube is pressed into shape by an upper and a lower tool.
    I modeled a non-linear material behavior for the pipe. Unfortunately, I was only able to solve the pressing phase from round into the desired shape after I reduced the Joung's modulus and the yield stress.
    *SOLID SECTION,ELSET=rohr,MATERIAL=cublech
    *MATERIAL,NAME=cublech
    *ELASTIC
    10e9,0.3
    *PLASTIC
    150e6,0
    160e6,0.01
    170e6,0.1
    200e6,0.91

    The tool movement is made by displacement constraints.
    t/s y/mm +- for upper and lower tool
    0 0
    0.5 2.5
    1 5
    1.1 4.9
    1.3 4.6
    2 1

    Now I wanted to see the condition when the tools are moved apart again. So the plastically deformed state on the pipe. Unfortunately I couldn't, because the solver did not solve and model "exploded"!

    Does anyone have sugegstions how to get such calculations running stable.

    Regards and thanks
  • VictorVictor
    These large deformations with contact can be finicky.

    It sometimes helps to turn off automatic time stepping and use a small time step.

    Also, make sure the pipe is fully constrained, perhaps at its other end, so that when the contacts let go, it's won't experience rigid body motion.
  • rwhirleyrwhirley
    Agree - these problems can be challenging (but fun!). A few thoughts:
    1. Set the pipe elastic modulus and yield stress to the desired values. Set the tool to be elastic with elastic modulus ~2X that of the pipe. This usually makes the contact work better than more mismatched moduli. Adjust the tool stiffness as needed. It is usually easier to get things to converge with softer moduli; once you get things working you step up the moduli to real values (sounds like you know this).
    2. Agree with Victor - use manual time stepping. Auto time stepping often leads to too large a step when contact first happens. Plan ~50 time steps for the closure - maybe more. Get that working well before you try unloading. Make sure there is not excessive interpenetration of the tool into the pipe at the final step. If there is, increase the penalty factor on the contact. Excessive interpenetration will often make the unloading crash.
    3. Your graphics suggest to me that the contact search algorithm failed, but it may just be an unconverged state. Be sure your displacement increment over one time step is not more than about 20% of the smallest element linear dimension. This can be small, but it will save you a lot of headache in return for more computing time.
    4. Once you add unloading, first try a small unloading step - maybe plan 25 time steps to unload from peak deformation to a small gap. You might need more to get things working.

    Hope this helps.
    -Robert
  • HengreHengre
    Thank you Robert and Victor, I will try to continue ;-)
  • JohnMJohnM
    Mesh matters here. If you under-predict stresses, you won't activate the plasticity as soon, and you'll likely under-predict the plastic strain and the permanent set.
  • HengreHengre
    Hello JohnM can you please explain a bit more what you mean. Thx
  • JohnMJohnM
    edited December 2020
    If a mesh is too coarse, the peak stress will not exceed the elastic limit, you won't activate plasticity, and you won't get permanent deformation. Run your model elastically, note areas where the stresses overshoot the yield strength. Make sure you have sufficient mesh density in these areas.

    Take a look at this example.



    Try running this model with increasing mesh density in the notch and you will see how density affects the result.
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