General Mechanical

General Mechanical

Simulation of flange joint

    • ganobe12
      Subscriber

      Hi everyone, I am trying to reproduce the results of a paper in which they have simulated a bolted flange joint with a gasket by taking symmetry across the half gasket thickness. Frictionless contacts are assumed and nonlinear gasket behavior is modeled. For bolt tightening, a certain displacement value is applied on the bolt shank bottom to get the target stress value. Also bolts are tightened one at a time thus multiple time steps are defined.

      In the paper APDL is used while I am using Workbench as I have no experience with APDL.

      Following the paper I have created my model but when I initially solve the model after applying a displacement value on the first bolt only I am getting weird behavior of the joints. I have tried to model symmetry by applying a frictionless support instead of a defining a symmetry region but in both cases I am getting the same issues:

      1)Some sort of rigid body motion/contact separation as all the bolts other than the one on which displacement is applied become separated from the flange after the 2nd step.

      2)Also large stress values are there in the 1st step which should not be the case as no load is applied in the first step. Only bolts are constrained in the radial direction. I am applying the displacement in the 2nd step only.

      I am attaching my ANSYS project file and reference paper here.

      I do not have too much experience with FEA thus any help would be much appreciated. Thank you

    • peteroznewman
      Subscriber
      I have added some constraints that allow this first step to be solved.
      It would be better to fix all the bolt faces at the center plane. Delete the displacement on the one bolt to tension it. Replace that with Bolt Pretension Load. In that way you can have 16 load steps. Step 1 is to load bolt 1, step 2 is to lock bolt 1. Step 3 is to load bolt 2, step 4 is to lock bolt 2, etc.

    • ganobe12
      Subscriber
      Thank you for replying peter however I am unable to open the file that you uploaded. I believe you saved the file using the latest version of ANSYS while I am using ANSYS 2020 R2 version.
      If possible kindly reupload the file using a previous version of ANSYS. Thank you
    • peteroznewman
      Subscriber
      Unfortunately, I only have a full license for ANSYS 2020 R1 and the Student license I use for ANSYS 2020 R2 does not let me edit the geometry.
      You need to open DesignModeler, use Explode Part on the Bolts part. Pick the four Bolt 1 bodies, then Form New Part. Repeat that 7 more times. Now you have one part for each bolt instead of one part for 8 bolts. That will let you do Bolt Pretension. If you do that, you can attach a new archive since I won't need to edit the geometry again.
    • ganobe12
      Subscriber

      I was able to open the project file you provided by installing latest student version of ANSYS.

      I have a question regarding that. Why are there large stress values in the first step as only constraints are applied in this step ? Load or displacement is applied from the second step. I should be getting minimum stress values in the first step and then the stress should increase as bolt is tensioned . Could you please clarify that ?
    • ganobe12
      Subscriber
      Also regarding your Bolt Pretension Load suggestion, I have some confusion.. please clarify the following

      1) How would I include symmetry of the bolts as I am modeling only half the length of the bolt ? Should the applied bolt load also be reduced to half ?
      2) In my model each of the bolts are divided into 4 parts. While trying to apply bolt pretension I am only able to select one of the four faces of the shank of a bolt. How should I select all the faces of the shank for bolt pretension ?
      3)Does the location of the applied bolt pretension matter ?? As while using bolt pretension, ANSYS automatically applies the bolt pretension at the center of the shank. While originally I was applying displacement on the bottom face of the shank.
      4)Also shouldn't bolt pretension be applied at the lower end of the shank as that would be the center if I had modeled the full length of the bolt ??
    • peteroznewman
      Subscriber
      1) It depends on how you define the load. If you define the load by a Force, then no, the force for the full length bolt is the same as the force in a half length bolt. If you define the load by a displacement, then yes, use half the displacement of a full length bolt on a half length bolt (to get the same force).
      2) I believe that after you use Shared Topology, you only need to select a single cylindrical face, and the Bolt Pretension feature will cut through the entire bolt. That is what I was hoping to learn by editing the geometry, which I could not do on the Student license.
      3) The location of the bolt pretension will be halfway along the cylindrical face you selected. That is fine as long as there are at least two elements along the length.
      4) It doesn't matter where Bolt Pretension cuts the shank, the force generated is the same.
      From your previous post, the stress in Step 1 is coming from the Offset you used on the Bolt Holes to Bolt Shanks frictionless contact. Set that back to 0.
    • ganobe12
      Subscriber
      Thank you so much for clarifying my queries.
      I am attaching the archive file with geometry already modified so that I have one part for each bolt.
      Also I have one more question. kindly clarify this one too if possible
      1) If I were to continue to apply bolt preload through displacement condition as was the case in the first archive file, then which stress result should I plot in the solution portion to verify if the given displacement value has created the desired pretension in the bolt ? Are the von-Mises stress result enough to verify if the target bolt stress has been reached or not??

    • peteroznewman
      Subscriber
      Simply insert a Probe of the Reaction Force of the Displacement. That will tell you the preload force in the bolt.
    • ganobe12
      Subscriber
      ok..
      And one more thing, when I try to use bolt pretension tool to preload the bolt, by selecting one face of the shank only, it creates pretension only in that part instead of the whole bolt. What can I do so that whole of the bolt is pretensioned ?
      I have already modified geometry so that I have one part for each bolt as you suggested before but still facing the same issue. Kindly further guidance is required. Thank you
    • peteroznewman
      Subscriber
      I don't slice my bolts into 4 pieces so I didn't know how Bolt Pretension would be applied.
      You have to apply four bolt pretensions, one for each quarter. After you define the first one, just use Duplicate and change the Geometry to a new face.
Viewing 10 reply threads
  • You must be logged in to reply to this topic.