General Mechanical

General Mechanical

Tubing convergence

    • zjuv9021
      Subscriber

      Hi all,


      I'm working on rotating part of a tubing 30 degrees, and then displacing the tubing as it hits a wall above it and slides past the fixed support and buckles (please see attached .wbpz labeled "Skin restriction"):


       



      I'm having difficulties getting this to bend to 30 degrees, let alone displace back through the tubing.


      Refining the mesh further seemed to make matters worse in regards to converging... so I'm a little lost. 


      Could anyone provide some demonstration on how to actually get this object to bend 30 degrees and slide past and buckle the fixed support?


      If possible, how would I set this up in Explicit Dynamics? Can this be done? I'm new to explicit, so any demonstration on how best to get started within there is greatly appreciated.


      Regards,


      Zach

    • Sandeep Medikonda
      Ansys Employee

      Zach, Didn't peter help you with this? How is this different?


      If your problem is with buckling of the tube. Note that buckling is a numerical instability, you would either have to add stabilization energy (energy-preferred) to your model or use the arc-length method (will need to use command snippets) in static structural. Please look up in the manual on how to do this.


      Regards,
      Sandeep

    • zjuv9021
      Subscriber

      Thank you, Sandeep.


      This is a little different. I have altered the geometry a bit and have included nonlinear Mooney-Rivlin 2 Parameter hyperelastic materials into my model.


      Regards,


      Zach

    • peteroznewman
      Subscriber

      Zach,


      I ran your attached model and it completed step 1, which was to bend 30 degrees, but it had a kink at the end of the tube and lost convergence during the push. I would make two changes.


      (1) I recommend instead of 50 elements along the sweep...



      ... using 200 elements along the sweep. This will be more stable, though it will take 4 times longer for each iteration.



      (2) How committed are you to rotating the "Tissue" tube about the end point...



      ...as opposed to rotating about a point between the fixed support and the opening of the tube?



      I think rotating about this point will give you a gentle bend that will have a better ability to form a loop that will later buckle where you want it to.


      I haven't run any of these changes, they are just my best guess of the direction of goodness.


      Regards,
      Peter

    • zjuv9021
      Subscriber

      Thank you, Peter. The rotation of the tube about the end point is not important, the mechanism of sliding up against the wall past the fixed support and buckling IS. I will try to move the point of the rotation to about halfway between the end of the "Tissue" and the fixed support.


      Kind Regards for all your help.


      Zach

    • peteroznewman
      Subscriber

      Zach,


      All the materials in the E system "Skin restriction" have only Isotropic Elasticity. I didn't see any Hyperelastic material properties in any of the material.



      I ran the suggestions above last night. The solver stopped at 90.4% of the way to 30 degrees, but had a uniform bend.


      The other change I made was the original model had warnings about small sliding may be violated.  Since this contact setting was Program Controlled, I changed all the Frictional contacts to have Small Sliding Off.


      You have a four layer tube inside a rigid tube. The four layers are shown below.



      The two outer layers are bonded, then the inner layers have frictional contact. 



      Contact failure of the two inner layers to each other and of the PET to the PU 80A is responsible for the convergence failure.



      How important to your model is it that these two inner layers have sliding contact?


      Here is the Silicone to PET contact that failed.



      Here is PET to PU 80A that failed.



       


      Error messages describe highly distorted elements, and element turning inside out. 


      I see you have Stabilization turned on.



      Here is the deformation on the last converged substep with the outer two layers hidden.



      Below is the unconverged result.



      I recommend changing the formulation of those two contacts to Pure Penalty, setting the Normal Stiffness Factor to 1 and the Detection Method to Nodal-Normal To Target.


      It took 2 hours and 42 minutes to compute to this point on 8 cores.


      I hope Sandeep can offer some suggestions.


      Regards,
      Peter

    • Sandeep Medikonda
      Ansys Employee

      Peter, try with a slightly higher energy dissipation ratio, use 1e-002. See if that helps? Looks to me that it was buckling based on those images.


      We can always monitor the Stabilization Energy vs Strain Energy and see how valid the results are if this helps complete.

    • peteroznewman
      Subscriber

      Thanks Sandeep,


      A second look at the model let me notice that a pressure load is applied to the inner surface. Currently, the pressure is being increased while the tube is being bent.


      It might be better to have a three step solution, where the pressure is applied in step 1, the tube bent 30 degrees in step 2, then the 4-layer tube advanced along the rigid tube.

    • peteroznewman
      Subscriber

      The changes I made let the model advance to 92% of step 1, but it now took 4 hours and 28 minutes. 
      I didn't get Sandeep's higher energy dissipation ratio in since it was already running when I read that.
      Here is the convergence graph.



      It didn't stop, I interrupted the solution since five bisections pretty much means it's not going any further.


      Here are some errors near the end:



      Maybe a hyperelastic material model and reduced order element integration will help this model converge.
      I will wait to see you implement that Zach and you should start a new discussion for that new material model.


      Regards,
      Peter

    • zjuv9021
      Subscriber

      Hi Peter - 


      Are you referring to Uniform Reduced Integration (URI)? I have never applied this and don't know the commands, so some assistance with how to implement is appreciated and then I will run. Is this keyopt, matid, 6, 1  on bodies I would like reduced integration performed on?


      I will start a new post with hyperelastic material in the meantime.


      Regards,


      Zach

    • Sandeep Medikonda
      Ansys Employee

      You can just insert that under the hyperelastic body in the Geometry part of the structure tree. For SOLID185, this is keyopt(2)


      keyopt,matid,2,1

      I think if you take what peter suggested and use some higher artificial/stabilization energy, it will push through since it is towards the end.


      Regards,
      Sandeep

Viewing 10 reply threads
  • You must be logged in to reply to this topic.