General Mechanical

General Mechanical

Bolt Pretension Analysis shows unrealistic stress

    • Rook207
      Subscriber

      I've been fighting with this project for months now and it's coming to a head now that I've verified my theory work with the CAD work. The gimmick is that the design aspect is only functionally correct due to the lack of specific details entailing thread pitch and so on. The issue I have is that the stress curve along the bolt length axis has a parabolic curve instead of one that would be best described as an elastic-perfectly plastic curve style. Given that the bolts stick out of the bottom of the pressure vessel plate ring, they should be experiencing the lowest stress on the free end since it has the most opportunity to deform.

      I've attached pictures and the zip files below, thank y'all ahead of time for looking into this one. My theory answer is matlab code specifically targeting deformation and with the forces involved should be ~0.2mm give or take 0.05mm.

    • peteroznewman
      Subscriber
      This model has 32 bolts. Suppressed Force loads are applied to the circular face, so this model has symmetry in both the geometry and the loads.
      This model has 31 too many bolts. In SpaceClaim, make two planes through the center axis with an angle of 360/32 degrees between them to straddle one bolt. Use Split Body to get a thin slice of the cover and flange. Delete the other solids and bolts. Do the analysis on one bolt.
      The bolt threads into the pressure vessel flange. Split the bolt shank face at the plane between the vessel and cover. The bolt shank face on the head end gets a Bolt Pretension. The bolt shank face on the vessel end gets a Frictional Contact to the vessel hole. Use a Contact Geometry Correction of Bolt Thread.
      Make sure to put at least 4 elements per thread pitch. In this example, use 1 mm element width along the bolt axis where the bolt threads exist.
      This shows more stress is in the first few threads, diminishing along the length and there is no stress in the end sticking out of the flange.
      Here is the full mesh. A Frictionless support is put on the two faces on each side of the 1/32 slice of the cover. A Z=0 constraint is needed on the Vessel. I choose the bottom edge.
      Good luck!
    • Rook207
      Subscriber
      Interesting, I tried slicing it but lacked the skills in spaceclaim to adjust it. I initially tried a symmetry-based system to represent the 32 bolts and went in way over my head haha. Did that study still represent the same deformation? I'll take a stab at it with this similar set-up, but that mesh looks highly dense and I'm using just the student version. I also didn't get any details from the paper I'm modeling on thread information, but I'll try your numbers and see how it comes out.
    • peteroznewman
      Subscriber
      I solved that model on the Student version. The way to create the two planes in SpaceClaim is to turn on the plane tool and click on the Coordinate System at the center. That will get you a plane through the center of one bolt. Then use the Move tool on that plane and click on the curved arrow to rotate the plane. Type in 360/64 for the angle. Now use the Move tool again but hold down the Ctrl key to get a copy and rotate that by -360/32.
    • Rook207
      Subscriber
      So you managed to get less than 32k nodes and elements? 1mm on the threaded portion and ~4mm generic size mesh goes above 60k for me. I must be misunderstanding how your mesh is developed.
    • Rook207
      Subscriber
      Thank you btw for all your help, you've been a saint so far!
    • Rook207
      Subscriber
      Actually, got the mesh down, but it isn't liking my constraint equations (fixed bottom of pressure vessel, rough between vessel and closure mass, frictional on bolt with vessel). I added a frictionless connection between the upper part of the bolt and closure mass, not sure what's happening but I'll dig through troubleshooting.
    • peteroznewman
      Subscriber
      For more than a year, the node/element count limit has been 128k. The 32k limit was abandoned around V2020.
      If you want to attach another .wbpz file, I will take a look. Say what version of ANSYS you are using in your reply.
    • Rook207
      Subscriber
      2022 R1 Student Edition, I must've found a bad source then, here's the file, meshing is fine now and they're structural steel until I get my constraints right, it's probably something really simple that I'm overlooking.
    • peteroznewman
      Subscriber
      You forgot to put a contact between the bolt head and the cover.
      You don't have two Frictionless Supports on the two faces that are the cuts for the pizza slice.

Viewing 9 reply threads
  • You must be logged in to reply to this topic.