Object collision

Yellow_clothYellow_cloth
When I do a 3D static analysis of an object that has some elements "inside" another set of elements, think of a multi-wall cylinder object, under application of internal pressure the deformation is, as if the "outer wall" isn't even there. Is this an issue, or did I overlook something?

Comments

  • VictorVictor
    If I understand you right, it sounds like they're not connected together. You can use Bonded contact for that.

    If they're supposed to be initially separated but come into contact when the pressure is applied, then you need a nonlinear analysis with Contact which requires the CalculiX solver. You would also use this if they might slide against each other.

    Let me know if you want more details on how to proceed. It might also be helpful to see the .liml file or at least a screenshot.
  • Yellow_clothYellow_cloth
    They're meant to be initially separated. I'll try the "Nonlinear Static 3D" analysis. But I would like more details on how to proceed. I'm not sure what the convergence criteria should be set to.

    Also, since Nonlinear Static 3D requires elements of a different type to what my geometry consists of (tri6), is there a way to convert the STL mesh to, for example, the type "tet4", by using NGsolve, or something?
  • VictorVictor
    You'll need to use the CalculiX solver for that.

    1) Download and install it as described in Chapter 14. You can get it from bConverged

    http://www.bconverged.com/data/content/CalculiX_2_10_win_002.zip

    or ddfem which is easier to sets up because it's a single binary.

    https://github.com/ddfem/ccx_mingw64


    2) Add contact between the two parts. See the sample file PipeClip.liml

    Tri6 shell elements work with the CalculiX solver so there's no need to change them. If you do want to convert them to solids, use Mesh tools -> Automesh 3D.



  • Yellow_clothYellow_cloth
    edited August 2016
    The PipeClip.liml example using the Calculix solver worked well. The ddfem version didn't run/install for me, but the bConverged version was easy to setup for solver association.

    I'll upload an image of a case using my own Tri6 geometry, since I'm not sure it gave the right results.

    Thanks for your help.
  • SergioSergio
    Is always good to check if the installation is working ok, on the bConverged start menu there is an icon to run a set of standard automatized tests.

    A few weeks ago I start to have wrong results, and after a lot of headaches I found that the problem was refered to the system variables, but I was able to be sure of the results only doing that autochecks.

    Regards!
  • davefodavefo
    Sergio

    What do the autochecks do? is a report provided verifying that all the autochecks have passed?

    Dave
  • SergioSergio
    It will run a set of standard problems and checks against know results, then inform you of any discrepancy. In Windows normally there are very few test with slightly different results, but I have an installation that give me almost all results different, and was due to the use of manually adjusted environment variables.

    I start to have some problems to run some analysis that I know that should run, then other problems gives me obviously wrong results, so then I start to investigate how to check the accuracy of the solver.

    So, be advertised :-) :-) :-)

    Regards!
  • Yellow_clothYellow_cloth
    This is an image of what I'm getting. It's not what I want. The colourful protrusions are the elements of the most inner cylinder. The pressure applied is only to that cylinder, but all the cylinders have a fixed support.

    The outer cylinders should have stopped the "protrusion", but the inner cylinder cuts through them like they aren't even there.

    What's wrong? What do I need to do?
    Regards
  • VictorVictor
    It looks like you haven't added ontact (CCX), which is under Loads & Constraints. You need to use that to explicitly tell it which surfaces might contact each other since it defaults to ignoring contact otherwise.
  • Yellow_clothYellow_cloth
    edited August 2016
    It's a bit difficult to add contacts to the faces since the cylinders are so close to each other, and this is a single model STL mesh, so I can't "hide" individual cylinders.

    But I got around the issue. It was quite complicated. Even then, the results don't seem to be right. Maybe. Because, the inner cylinder cut through the outer cylinder, but the outer cylinder warped a bit (by a very little amount).

    This image is of a model with only two cylinders.
  • VictorVictor
    Penetration is unavoidable with this type of contact. You just have to reduce it to an acceptable level. Do that by increasing "Slope of pressure-overclosure curve K", perhaps by an order of magnitude at a time until the penetration is acceptable.

    I notice it seems to have long thin triangle elements. These are probably not very accurate. If it's a closed STL surface, you could use Mesh tools -> Automesh 3D to remesh it with better shaped elements.

  • Yellow_clothYellow_cloth
    edited August 2016
    It worked.

    I changed the "Slope of pressure-overclosure curve K" in the contact parameters from 2000 GPa/m to 20000 GPa/m.

    The only issue with remeshing is that Netgen/ngmesh says it cant do it, because there are too many trig neighbours or something. But I can get that fixed with netfabb (most of the time), or I can just do a simple x2 refinement.

    But I'm happy with what I've got here.
    Thank you.
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