General Mechanical

General Mechanical

Frictional Contact Penetration Problem

    • samuelchrist

      Dear Ansys Community,

      I am trying to simulate contact between Polyurethane Disk and the inside of a Steel Pipe in order to measure the frictional force experienced by the disk. The model that I use is Axisymmetric 2D. The problem that I constantly face is that the disk penetrates the thickness of the steel pipe even though the contact between the two is defined as Frictional with a friction coefficient of 0.4


      Any suggestions to solve this problem? The link below is the Ansys project file.


      Ansys Project File + Penetration Picture

    • Aniket
      Ansys Employee

      ANSYS employees are not allowed to download files from the student community, so hopefully, others can help in this regard.

      If you want to reach a broader audience, kindly insert the images inline in your post instead of external links.

      Generally, the Friction coefficient does not affect penetration. It will affect the force that is required for sliding the two parts together.

      How much is the penetration? If the contact is detected and you want to reduce the penetration in the contact you will need to increase FKN i.e. Normal stiffness of the frictional contact.


      Guidelines on the Student Community

      How to access ANSYS help links

    • peteroznewman

      Dear Samuel,

      I opened your axisymmetric (Y axis) model.

      The problem in your model is that you have assigned an X=0 displacement to the entire top edge of the pig.

      The pig cannot compress except on the radius with that boundary condition.

      I suggest you make the following changes to the model.

      • Delete the Fixed Support and the Displacement BCs.

      • Add a Frictionless Support to the top edge of the pig.

      • Add a displacement BC to the outer edge of the pipe, X = 0 and Y = 5 mm

      • Turn on Auto Time Stepping

      • Set the Initial Substeps and Minimum Substeps to 100

      • Add a Command to Static Structural to make it keep iterating for longer than 26.     NEQIT,100

      • Increase the Mesh to Resolution 3

      • Change the Contact Normal Stiffness back to its default value of 1

      Now the pipe will move up and the pig is free to be compressed but that is not enough. The convergence stops after 1.25 mm.

      One way to help it converge is to draw a more gradual compression profile on the pipe entrance. Another way is to add a remote displacement to the end of the pig to compress it, then move the pipe up then deactivate the remote displacement. I have done a part of this below, but I haven't put it all together.

      I expected a pig to be a much longer object, but perhaps this is just the scrapper and there is a much longer carrier that keeps it aligned in the pipe.


Viewing 2 reply threads
  • You must be logged in to reply to this topic.