General Mechanical

General Mechanical

Convergence during Large Deflection of Hyperelastic Materials

    • peteroznewman
      Subscriber

      Here are my five must do items to achieve convergence in hyperelastic material undergoing large deflection.



       


      ANSYS 2020 R1 archive attached

    • Amin1372
      Subscriber
      Hi Peter,nI need to use Silicon rubber in my Ansys workbench model and I did exactly what you said including: n1) Using Silicon Rubber with mooney rivlin 2 parametern2 & 3) Writing these commands: nKEYOPT,matid,6,1nKEYOPT,matid,2,1n4) Generating a good mesh with more than four elements through the thickness of the part made of Silicon rubbern5) Taking many substepsnnnbut I got this error:nn*** ERROR *** CP = 2.859 TIME= 01:58:37n For element type = 11 (SOLID187), KEYOPT(2) = 1 is invalid. nwhat should I do?.Thanksnn
    • peteroznewman
      Subscriber
      Take out that Keyop, it doesn't exist for SOLID187, a quadratic tet element.nThat keyop is for SOLID185, a linear hex element.nYou might get better convergence with SOLID185 than SOLID187.n
    • Amin1372
      Subscriber
      Hi,nHow I can change the element to SOILD185 in workbench?n
    • Amin1372
      Subscriber
      nPeter can you please take a look at my simulation to check whether it can be converge or not? I will really appreciate you.nThanks n
    • peteroznewman
      Subscriber
      You get SOLID185 elements by setting the Mesh Details to have Element Order = Linear instead of Program Controlled, which is often Quadratic.nYou get Hex element shapes instead of Tet element shapes by slicing the geometry into six-sided solids and using mesh controls like Sweep and Multizone.nI looked at your model and it has some problems. There is a large overlap of the tooth with the Silicone Rubber. You may have better luck with a multistep solution where the teeth start out tangent to the rubber and bite down on the rubber, then any other loads are applied in step 2.nn
    • Amin1372
      Subscriber
      I changed the Element Order to Linear instead of Program Controlled and defined Hex element shapes, but I tried PC+Plastic for tray before using Silicone rubber. So I didn't apply those items to achieve convergence in hyperelastic material. In addition, I changed the tray to a flat one without any profile to avoid the overlap of the tooth with tray and just defined 1mm interference at the interface of the two teeth (number 2 & 7) and tray. nThe results of the reaction force were so odd because the applied static force was 0.3 N and the reaction of the tooth number 2 was about 2000 N. Could you please help me to fix this problem? Thanksnnn
    • peteroznewman
      Subscriber
      The size of an applied load far from the interference of the tooth is irrelevant.nIt is perfectly understandable for the ABS+PC Plastic material that 1 mm of interference generates 2000 N of reaction force. To check that this is reasonable, use F = A*E where E = 2510 MPa. If A = 1 mm^2, you would expect 2510 N of force. Silicone rubber is much softer than ABS+PC.n
    • Amin1372
      Subscriber
      Hi Peter,nYes you are right, that's understandable for ABS+PC to generate this reaction force but for Silicone rubber is not reasonable as I got the same results. Does it have any other reasons? I would really appreciate if you help me to solve this solution because I am missing a deadline.nn
    • peteroznewman
      Subscriber
      It is more reasonable to assign a force that the teeth apply to the plastic, rather than a displacement. That way if the material is stiff, the displacement is small and if the material is soft, the displacement is larger. I think human bite force would be a known statistic in the human factors literature.n
    • Amin1372
      Subscriber
      I understand what your saying but in my case I am looking for the force distribution on the teeth when the static force is applied on the tray. And the reason for using interference is to see its effects on the reaction forces. nBut I still have problems and no progress, can you provide me a recommendation?nThanks n
    • lgerez
      Subscriber
      Dear Peter,nThank you very much for the detailed tutorial about hyperelastic structures. I followed your suggestions but I still can't make my simulation to converge (the Keyops did not change the force convergence plot). I am trying to simulate the inflation of a silicone rubber structure by applying pressure to the internal faces. The mesh has good quality in general (I've tried several mesh sizes and shapes) and the boundary conditions are well defined. Do you have any further suggestions for improving the model?nThank you very much,nnLucasn
    • peteroznewman
      Subscriber
      Dear Lucas,nA couple of suggestions.n1) This is an axisymmetric problem. Use a 2D surface body and an Axisymmetric analysis.n2) You didn't get the Keyopts quite right. The most important one is Keyopt(6)=1.nI would have tried the 2D model, but unfortunately, the mechdat file doesn't include the geometry file.nRegards,nPetern
    • peteroznewman
      Subscriber
      I didn't see how far your model went as provided. When I just apply 2) and also turn on Stabilization (Nonlinear Controls under Analysis Settings) this is what I get. Convergence stopped at 51% of the load. Here is the initial shape.nRegards,nPetern
    • lgerez
      Subscriber
      Hello Peter,nThank you for your quick reply. nI will try to use a 2D surface body and an Axisymmetric analysis as you suggested. Regarding the Keyops, I tried them separately and also employing both of them in the same command and in both situations my simulation stopped approximately at the same stage. nHopefully I attached all the correct files this time nRegards,nLucasnArrayn
    • lgerez
      Subscriber
      Hello Peter,nMy convergence also stops at 51%. The motion of the center part is not important at this point of the study, so I inserted a hole in the center so I could have a better mesh and simplify the analysis. My plan is that once this simplified version of my setup works well in simulation I incrementally add the other features.nRegards,nLucasn
    • peteroznewman
      Subscriber
      The highly distorted element error message stops to the solution from proceeding much further than 51% of the way to 8e-2 MPa (11.6 psi). I pulled the flat to the axis so there is no hole in the flat.nI don't know why you have such a thick elbow on the flat. If you resize the dimension on the lower arc of the elbow to 2 mm, then you get a uniform wall thickness and there is no highly distorted element problem.n
    • peteroznewman
      Subscriber
      Maybe less of a highly distorted problem. I wrote the last line and later discovered that the pressure load was no longer on that arc, which is why it solved to the full load. I am now trying to get a solution to the full load with the pressure along the entire inside face.n
    • peteroznewman
      Subscriber
      nOne idea is to try Explicit Dynamics, but you will have to define the Incompressibility parameter D1 on the material model before that will run.n
    • peteroznewman
      Subscriber
      n76% of the way to a pressure of 8e-2 MPa using Explicit Dynamics. The other required material parameter is Density. I made up a number for density, just like I made up a number for the D1 incompressibility parameter, just so I could click the Solve button and have Explicit Dynamics run. If you use this solver, you will want to put in real values.nThis is a Dynamics solution, so the time over which the pressure ramps up from 0 to 8e-2 MPa matters. This shape is what you get when you ramp it up over 0.1 s but you would get a different shape if you ramped the pressure up over 0.001 s or 10 s.nn
    • lgerez
      Subscriber
      ,nThank you for the suggestions. I was able to successfully run the simulation employing a 2D Axisymmetric analysis, as you suggested.Thank you!nn
    • Mojish
      Subscriber
      ,nThank you for your helpful tutorial on the simulation of hyperelastic materials. I am trying to run a simulation of the compression of a circular silicone rubber band made out of RTV615 constrained by two shafts, but I've been struggling to make the simulation to converge. I've followed your tips but the simulation still fails at less than 20% of the way. The rubber band is not symmetric so I believe I cannot interpret this problem as a 2D problem. Do you have any suggestions on how to improve it?nRegards,nMoji nn
    • peteroznewman
      Subscriber
      nI ran your model, but it only gets to 0.45% of the 10 N load or 0.045 N, which is much less than 20% of the way.nI made many changes, one was to replace the force with equivalent pressure. I don't know if that was necessary.nI got the attached model to solve to 3.1% of the load in 38 minutes on my 4-core computer. It stopped due to a highly distorted element. Further progress would be achieved by making many more smaller substeps, and possibly making smaller elements. One change I would make to the attached archive is on the Remote Displacement, make X free so that it can expand out to the outer face.nIt might be possible to get it to the full load in Static Structural, but the next phase is for the part to buckle and the material around the holes to collapse. That may be easier to simulate in Explicit Dynamics.n
    • peteroznewman
      Subscriber
      If you are trying to obtain a Torque-Rotation Angle curve for this, then it would be best to put in a Remote Displacement on the end face and Rotate that about the center. That way, you can recover the Torque when you Probe the Remote Displacement.nWas this part molded in a cylindrical shape? Some parts like this are molded flat, then rolled up and inserted into a cylindrical space like you have. A flat part that is rolled up has a different pattern of stress in it as it gets squeeze in rotation than a part that was molded in a cylindrical shape to begin with.n
    • peteroznewman
      Subscriber
    • Mojish
      Subscriber
      Hello Peter,nnThank you for your comprehensive reply. This part is molded flat, then rolled up in a cylindrical space, but I have no idea how should I take it into consideration in my model.nThe video shows exactly how it is supposed to move. For the density, when I reduce it to the right amount, it takes a couple of hours, then it stops due to a highly distorted element. I will try smaller sub steps and elements as you suggested. nThank you so much.n
    • peteroznewman
      Subscriber
      Hello Moji, nThe density is only relevant for Explicit Dynamics.nThe following steps work in Static Structural for a body with a uniform cross-section. It may not work so well for a part with large holes in it.nIn CAD, create the flat solid, place the fixed end in the cylindrical gap and let the other end poke out.nIn Static Structural, define the wall contacts, a remote displacement on the moving end face, a pressure load and create a multi-step analysis.nIn Step 1, the contact with the wall is Inactive, the pressure is zero.nThe flat hyperelastic part has the end fixed, which is located in the cylindrical gap. At the other end, a Remote Displacement applies a rotation about Z to that face, leaving the X and Y translation DOFs Free. For a uniform plate, that will curl the object into a circular shape during step 1, and the part would be in the cylindrical gap. You won't get that due to the holes.nIn Step 2, contact with the cylindrical walls is made active. If there is some small penetration of the part through the walls due to the non-uniform nature of the part, the contact might successfully resolve that in step 2.nIn Step 3, the remote displacement constraint is made inactive, the part will uncurl until it touches the wall.nIn Step 4, the pressure increases from 0 to something.n
    • Emperor
      Subscriber
      thanks for the tutorial which is useful. I am working on a nonlinear structure in static analysis (I have detailed some elements here, and I have already been able to solve these problems). I would like to know if it is not possible to apply the hyperplastic material on the solid285 with a quadratic order?! I am currently running the 9 step simulation and I have an error at step 6 (see video below). Do I have to use the linear element?.
    • Emperor
      Subscriber
      sorry, I forget the video : nn
    • Emperor
      Subscriber
      I saw that solid185 and a hexa element, so I can't apply it to my elastomer which is tetra meshed, do you have any suggestions please?n
    • andrea giordano
      Subscriber

      Hello Peter, 

      what if one does not have an axis symmetric domain? 

      Thank you very much!

      Andrea

Viewing 30 reply threads
  • You must be logged in to reply to this topic.