General Mechanical

General Mechanical

Shell slide on rigid body

    • bokaJ
      Subscriber
    • peteroznewman
      Subscriber
      nDelete the Fixed Joint, Body-Body.nInsert a Fixed Joint, Body-Ground, and select only the Rigid Body.nInsert a Contact between the Rigid Body and the 11 faces of the floor of the structure. The Rigid Body face must be on the Target side. Make the Contact type be Frictional or Rough. A rough contact will not slide on the rigid body, but can separate. You want to see the blue color on the opposite side to what you show in the image above. You do this by setting the Contact Side to Bottom instead of Top.nUnder the Connections folder, insert a Contact Tool and Generate Initial Contact Status. The Frictional or Rough contact must show as Closed. nUnder Analysis Settings, turn on Auto Time Stepping. Set the Initial Substeps to 100.n
    • bokaJ
      Subscriber
      nThank you very much for your quick and very helpful answer.nAs you can see in the following picture, the deformation looks as expected.nnBut there is a slight step through at some areas. In my opinion this should not be possible?nOn the picture below, you can see the details of the contact between the rigid body and the shell body.nOn the picture below you can see the initial information of the contact. nFor the hickness of the shell and the rigid body I choose 15mm. But I put the rigid body directly on the shell, or should I leave a gap of 15mm(=7,5+7,5) between the shell and the rigid body?nWould you possibly so kind as to help me again with this problem?.Thank you a lot,nbokaJn
    • peteroznewman
      Subscriber
      nYou can either put two surface bodies on the same plane and leave Shell Thickness Effect turned off, ornyou can put the two midsufaces 15 mm apart and turn on Shell Thickness effect.nIn either case, the thickness assigned to the surfaces is 7.5 mm.nContact algorithms allow a very small penetration to be used to compute the contact force needed to prevent large penetration. You can control the size of that very small penetration by altering the Normal Contact Stiffness Factor. The default value is 1, you can increase it by a factor of 10 or 100.nYou can insert a Contact Tool on the Solution branch and insert a Penetration plot on that tool. That will show the value of penetration as a contour plot. Note that the Deformation Result is often scaled to look 1000 times more that reality. Set the Result Deformation Scale to 1.0 (True Scale).nhttps://forum.ansys.com/discussion/14332/deformation-scalen
    • bokaJ
      Subscriber
      thank you very much sir!nthe maximum penetration is about 0,001mm.nI learned a lot from you!nnBest regardsnbokaJn
Viewing 4 reply threads
  • You must be logged in to reply to this topic.