General Mechanical

General Mechanical

Balloon with ball contact

    • F. Semih Y
      Subscriber

      I try to analyse the reaction forces on the ball from the expanded balloon. I get following messages:


      error: The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information.


      warning: The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.


      warning: Contact status has experienced an abrupt change.  heck results carefully for possible contact separation.


      Attached is the archive file. I am pretty sure the problem lies within the contact definitions/options. Please a rather personal solution applied for my file. I don't want to change a lot of advanced (mesh, contact, analysis) settings (pinball radius, integration point detection, surface projection contact detection) without knowing sure they are even a potential solution. If it is the case I do need to change some settings, please clarify how. Because the Simulation runs fine when the frictional contact 'balloon with frame' is changed to either bonded or no separation. This means that either the setup of that contact is wrong, or the ball contact. Because the balloon does not reach the ball when the above stated change in contact is applied. 


      Only specific changes i applied are: changing time steps and turning on large deformations. 


    • Sandeep Medikonda
      Ansys Employee

      Semih,


        I am unable to look at your file. But there are a few good discussions on this error in the forum that should help:


      Discussion 1


      Discussion 2


      One initial impression I have based on that image is that the mesh is way too coarse, see if refining it helps.


      Regards,
      Sandeep

    • peteroznewman
      Subscriber

      I recommend you create a Midsurface of the balloon. This will allow a much more robust shell mesh to be put on the midsurface. A shell mesh is assigned the thickness of the solid, but has the ability to bend that a solid element does not have.




      This kind of model is very difficult to achieve convergence because there is only a tiny change in equilibrium for large changes in deformation.


      Regards,
      Peter


      Sorry, I don't have AIM 19.0 installed, I have AIM 19.2 (archive attached) that you will not be able to open with AIM 19.0.

    • F. Semih Y
      Subscriber

      Mesh refinement was a solution. I applied local refinement to the contact surfaces. The simulation took 27 minutes. I also used a symmetry plane as explained in a previous topic:



      If you have quartered the CAD model, you can apply displacements to the cut faces to create the Symmetry BC that you need. If the model is entirely solids, then on a cut face whose normal is parallel to the Z axis, assign a displacement of Z=0 while leaving X and Y free. Similarly, on a cut face whose normal is parallel to the X axis, assign a displacement of X=0 while leaving Y and Z free.


      If you have midsurfaces, then you also have to constrain two rotations on the cut edges of a midsurface; the two axes that are not the zero displacement axis.


       


      Regards,
      Peter



      I'm still looking to improve the simulation time.


      I thought it would save a lot of computation time if I set the object (ball) as rigid. I only need the reaction forces at the surface after all. I don't know how to set them as rigid bodies though. If i import the bodies to mechanical app, I cant change the material properties or turn of 'flexible body'. 

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