General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

convergence problem – nonlinear material / plastic deformation

    • Joona

      Hello everyone,

      I'm trying to do a static mechanical simulation with two flanges and a copper ring (as a sealing material) between them. The two flanges are held together by six bolts which are having bolt pretensions (see image 1-2). Each bolt pretension is set to 10kN. The plastic deformation which is seen on the surface of the copper ring (nonlinear material) due to the bolt pretension is intended (see image 3). I always receive the error message "Internal solution magnitude limit was exceeded". I generated a finer mesh, reduced the times steps, did more load steps, but it did not work. I would appreciate if you could help me with this. Thanks a lot.


    • Aniket
      Ansys Employee

      From the images, it seems like the two flanges are passing through each other. The first thing to check is to check the contact status between the two flanges.

      Do check the following as well:

      1. Bolt pretension applied in 2 steps, first one loads, second one locks

      2. Any additional loads should be applied in third and subsequent steps

      3. bolt head should have bonded contact with flange and so does a nut and the flange

      4. check the initial contact status of the two flanges, they should have frictional or frictionless contact (not bonded) and the contact should be closed ideally


    • peteroznewman

      It looks like there are triangular ridges on each side of the copper ring.

      I would take each flange and separate the triangular ridge into a separate body so that body can have a structured mesh. You can use Shared Topology to connect the separate triangular bodies to the rest of the flange. There should be a radius at the top of the ridge and not a point (edge). You could split the copper ring so that you can put a higher mesh density under the radius of the ridge.

    • Joona

      Thank you for your answers!

      I will check the contact status and separate the triangular ridge into a another body, where I can generate a structured and finer mesh.

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