General Mechanical

General Mechanical

No elements in contact area

    • maetha
      Subscriber

      Dear all


      I am simulating the construction attached. If I'd like to solve the model, there is this error message aborting the calculation (originally in german): There are no elements in a contact pair area or in an external force. ...


      The problem is somewhere in the structural node on the top of the pillar. If I deactivate the 2 horizontal cylinders, the message disappears.


      Does somebody know how to solve this error?


      Thanks for your help!


       

    • peteroznewman
      Subscriber

      What version of ANSYS are you using?

    • maetha
      Subscriber

      This is ANSYS R18.1 Academic

    • peteroznewman
      Subscriber

      The error message in English suggests that the contact may have been defeatured away during automatic Mesh based Defeaturing. That can be turned off under the Mesh Details window.



      I did that and cleared and Generated the Mesh, but upon Solve, the error repeated, so that wasn't it.


      The contact that is experiencing a lack of elements can be found by opening the ds.dat file. If you highlight the Solution branch, RMB and select “open solver files directory”, you can locate the file. Scroll down to the end of the file. The last contact pair listed is the last one successfully created. The next one is the problematic one.  In your case, that would be this one:



      There are two joints with the same name. The first one shown below is working.



      The second one shown below is causing the error, which is confirmed by suppressing this joint and hitting Solve.



      Note that the coordinate system is not on the other joint. This may be the cause.


      For corrective action, I suppressed the second revolute and made a fresh revolute joint
      Now there is a reference coordinate system on that side. ANSYS 18.1 archive is attached.

Viewing 3 reply threads
  • You must be logged in to reply to this topic.