Static Structural analysis system failed

- February 12, 2019 at 11:14 am
  
  fx213
  Subscriber
  
  Hello,
  
  I would like to ask you a question on the analysis system of a static structural study that I tried to run on a cylindrical rubber sample but it failed.
  
  I have attached the respective file and I have also cited images of the Elastomer sample (Mooney Rivlin) [1] that I assigned from ANSYS Engineering data Hyper-elasic materials and the another one with all the steps of the analysis system.
  
  In the analysis settings, I inserted fixed support on the one cross-section (edge) of the cylinder and I applied displacement on the other cross-section (edge) of the cylinder in order to apply in that way axial compression stress on the model. I selected the result I wanted from the solution afterwards.
  
  Could you have a look and give me some feedback on where I have done wrong in the analysis steps or what I have omitted in that and it failed?
  
  Thank you in advance for your time.
  
  Kind regards,
  
  FX
- February 12, 2019 at 11:41 am
  
  jj77
  Subscriber
  
  Could you please attach the model (it is not attached).
- February 12, 2019 at 11:58 am
  
  fx213
  Subscriber
  
  I think that I have to save the file in .wbpz type, whereas when I try to save the workbench project schematic, the only option is to save it in *.wbpj.
  
  Any suggestion on how I can attached the file in the discussion?
  
  Thank you
  
  FX
- February 12, 2019 at 12:13 pm
  
  jj77
  Subscriber
  
  Go to file and archive, that will save it as .wbpz.
- February 12, 2019 at 12:42 pm
  
  fx213
  Subscriber
  
  Thank you.
  
  FX
- February 12, 2019 at 1:56 pm
  
  jj77
  Subscriber
  
  I would fit a 5 parameter MR, as the one par. is not representing the exp. data/curve really well (very bad actually).
  
  The main reason of the converg. issue is the large displacement applied, which is much larger than the whole cylinder, so of course it cannot solve.
  
  Apply something reasonable and use the 5 parameter MR, and then it is OK.
- February 12, 2019 at 2:11 pm
  
  peteroznewman
  Subscriber
  
  fx213,
  
  The cylinder is 11.18 mm tall, but the displacement is to compress it by 81 mm! That is clearly a mistake. I changed the displacement to -4 mm.
  
  Under Analysis settings, you must turn on Large Deflection
  
  Under Analysis settings, turn on Auto Time Stepping and set the Initial and Minimum Substeps to 100, the maximum can be 400.
  
  But that is not enough, it needs some more help in the form of Reduced Integration. Under Geometry, set Element Control to Manual, Under the Body, set Brick Integration Scheme to Reduced.
  
  I will post this now, even though with those changes, it stops converging at 0.18 mm. There are Keyop settings I have to go and look up, or perhaps a different element type.
  
  You could make this go faster if you took a radial slice and used a 2D axisymmetric model.