Resolving convergence issues between shell bodies and solids

I'm investigating the integrity of a MP under his self-weight. The contacts are all frictional between the rollers and the monopile. I've adjusted several things but it's never able to converge fully, only about half the weight is applied and it stops. Could anyone help me out?





Answers

  • peteroznewmanpeteroznewman Member Posts: 11,054

    @ArisvHouten

    Why did you increase the Normal Stiffness Factor to 5?

    Have you added 3 Newton-Raphson Residuals under the Solution Information folder? Where is the maximum value of N-R Force Residual?

  • ArisvHoutenArisvHouten Member Posts: 15

    Good afternoon Peter,

    Based on the Newton-Raphson Residuals when the normal stiffness factor was program controlled and updated every iteration. I observed a high spike in the contact between the rollers and the monopile. On top of that the penetration was at a value of 4.7 mm before it diverged. Thus, I took it upon myself to increase the Normal Stiffness Factor to 5 to avoid this penetration. As soon as the run is completed i'll add the new Newton-Raphson Residuals plots in this discussion, I did not save the old ones..

    My best regards,

    Aris van Houten

  • ArisvHoutenArisvHouten Member Posts: 15

    Please find the archived file attached. I can't seemed to get any convergence anymore...

  • peteroznewmanpeteroznewman Member Posts: 11,054
    edited January 9

    @ArisvHouten

    I can't run this model on the Student license since there are more than 32,000 nodes.

    Try flipping the contact and target definitions on all the contacts.

    Try increasing the Initial Substeps up to 100.

  • ArisvHoutenArisvHouten Member Posts: 15

    Thanks for you answer Peter,

    I tried both and it still could not converge..

    There are no spikes in the Newton-Raphson Residuals over 1.2N.

    Do you have any other suggestions, or maybe something in the contact formulation I should change?

    The only load present here is gravitational, but it still gives issues.

  • peteroznewmanpeteroznewman Member Posts: 11,054
    edited January 10

    @ArisvHouten

    There are many problems in your model. I found two surfaces at the same station on the tube. Get rid of the duplicate. You also did not use the Share function on the Workbench tab in SpaceClaim to connect different rings of the tube.

    I cut the tube in half to reduce the number of nodes so that it would run in the Student version. Doing this can help convergence. I also changed the roller material back to rubber because the very high pressure on the roller makes an isotropic material more difficult to converge than a hyperelastic material. I also changed the rubber elements to mixed u-P formulation.

  • ArisvHoutenArisvHouten Member Posts: 15

    Thanks a lot for your time, Peter! I really appreciate it.


    With regards to the share topology, for one model I did and this didn't resolve it. I notice that connecting the mesh with manual mesh connections generates a higher quality mesh normally. But this may not help for convergence. Unfortunately you need an Enterprise license for nonlinear rubber. Which is very scarce within our company, hence the face I've used Isotropic Rubber.

    Cutting the tube in half is not a possibility as other load cases shall involve momentum and accelerations in the X-direction.

    Did you change anything under the contact settings with respect to mine and under solver settings, that I must be aware of?

    I'm not aware of the mixed u-P formulation, is this under the Engineering Data settings?


    I'm awaiting your reply.

    Aris

  • ArisvHoutenArisvHouten Member Posts: 15

    Hi Peter,

    Could you share your archive version of the project. I changed everything according your suggestions, but still end up not converging..

    My best regards,

    Aris

  • peteroznewmanpeteroznewman Member Posts: 11,054
    edited January 11

    @ArisvHouten

    Note: the half model was a quick and dirty model. I did not take the time to make all the shell thickness values correct, they are all at 58.9 mm thick. I accidentally made the duplicate surface, that was not in your model.

    How far does your convergence get? You should show the N-R Force Convergence plot.

    I left the contacts at the default setting as created, with the rubber on the Contact side. There was up to 5 mm of penetration, but that will probably not change the stress in the tube if I turn up the contact stiffness.

    Mixed u-P formulation is in the ANSYS help system. You turn it on using keyop(6)=1 via a Command object under each roller body.

    Since you are on a Corporate license, you can get help from the Tech Support provider where the ANSYS license was purchased.

  • ArisvHoutenArisvHouten Member Posts: 15

    Hi Peter,

    This I did but still no convergence. Should I still decrease my step-size or something else?


  • ArisvHoutenArisvHouten Member Posts: 15

    The weird thing is that when I generate automatic connections. Its shows that there are still shells to be connected (1st figure). But I already shared the topology of all shells. If I check in SpaceClaim I do not see any duplicates however. Could this be because I used SpaceClaim 2019 and 2020?


  • peteroznewmanpeteroznewman Member Posts: 11,054
    edited January 12

    @ArisvHouten

    You don't have duplicate surfaces, I accidentally did that when I was splitting the tubes, as I mentioned above.

    Delete all the automatically created Contacts between the tube edges since you are using Mesh Merge (or Share button) to connect them.

    The frictional contacts all must have Adjust to Touch. I think this is why your model is not starting. I made a nice mesh on the rollers. I added very light spring to ground from the center of one end using a deformable connection to the edge, just in case the lack of an axial constraint was necessary. I could delete that and see if it was necessary.

    I replaced Standard Earth Gravity with Acceleration so that I could do a 2-step analysis. Note that the arrow has to point in the opposite direction!

    Step 1 took the acceleration up to 7 m/s^2 and has initial and minimum substeps of 10.

    Step 2 took the acceleration up to 9.81 m/s^2 and had initial and minimum substeps of 100. You can try 50. This was mostly to allow convergence on the rollers. It may not be possible to converge without using Hyperelastic Materials and the mixed u-P element formulation. I could switch back to the iso rubber and see if it can converge.

    Consider replacing each roller with a spring to ground. That way, there will be no convergence issue with the roller.

    Find out the name of your Technical Support provider for this Commercial license. You can get them to help you.

  • ArisvHoutenArisvHouten Member Posts: 15

    Thank you so much for your time and help, Peter!

    Adjusted to touch accompanied with the light springs did the trick!

    I'm in contact with my Technical Support now.


    P.S. The automatically created connections is because the tolerance value was that large (183mm). Reasoning that the model itself is large also.

Sign In or Register to comment.