General Mechanical

General Mechanical

How to solve nonlinear problem with rubber

    • Yun Wei Chuang
      Subscriber

      Hi everyone

      I am a new ansys workbench student, and the problem right now is the message with "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." I think that maybe something about engineering data for rubber or it could be contact faces, but model is too complex...

      I already turned "Large Deflection" to on, so what else steps I can do to figure out the erro? The model is about air sprin; the picture is down below. Plz help me.

      or perhaps I can send you file by email. Any suggetions could help.

      thank you

      Wayne Chuang

    • peteroznewman
      Subscriber

      Hi Wayne,

      I can help you with this. In Mechanical, click on Mesh and Clear Generated Data, then close Mechancial. In Workbench, do a File Save, then do a File Archive to create a .wbpz file.  Place that file on a sharing site such as Google Drive, OneDrive or Jumpshare. Paste the link to the .wbpz file in your reply.

      Regards,

      Peter

    • Yun Wei Chuang
      Subscriber

      Hi Peter

      I already created a file. => https://drive.google.com/file/d/1IrSRwUUSnsk7wyxb2Zdb8Ed3wKgKThud/view?usp=sharing

      I hope that could work. please check. Thank you for your help.

      regards,

      Wayne Chuang

    • peteroznewman
      Subscriber

      Hi Wayne,

      I got your file, opened it and will look at it today.

      It would be helpful if you also put the file 700T-1013.x_t into the Google Drive and send me a link to that so I can make geometry edits that will help the simulation.

      One idea is to create an Axisymmetric model of the air spring assembly.  That will only be useful if you are only interested in axisymmetric loads. It will not be useful if you want to tilt one side relative to the other.

      Regards,

      Peter

    • Yun Wei Chuang
      Subscriber

      Hi Peter

      Here is the soidwork file => https://drive.google.com/file/d/1r9g2-_KNRWepbb3LyWX4z1puo2XAtg8H/view?usp=sharing

      thank you again

      Regards,

      Wayne Chuang

    • peteroznewman
      Subscriber

      Hi Wayne,

      Is it useful to have a model that can only move axially and radially and can’t tip or tilt or move off axis?

      What information do you want to get out of this model?

      Is this profile you made the as-formed shape, or was it molded using a more open shape to begin with, as illustrated with the orange line, then when assembled to the parts it is forced to take on the shape you have drawn?

    • Yun Wei Chuang
      Subscriber

      Hi Peter,

      Right now I want to find vertical stiffness (Kz) like the picture below. After, horizontal problem will be considered. (Kx,Ky)

      For the geometry, orange line is 3D scanning original version. The samll parts such as nylon and steel, I add to the model.

      Maybe the powerpoint file can let you understand more.

      https://drive.google.com/file/d/16ty7HrgB57BZotzcgwKnBiFznxssi73p/view?usp=sharing

    • peteroznewman
      Subscriber

      Hi Wayne,

      I don’t understand the stiffness vs load graph. What is the difference between the red and black colors? What is the meaning of the lines vs the markers?

      I also don’t understand your reply on the shape you created in SolidWorks. Is that the as-molded shape before assembly or is it the deformed shape after assembly. Please clarify. For an FEA model, it’s best to use the as-molded shape before assembly.

      Many changes will help this model to run better.

      The geometry is cut in half, but there is no Symmetry Boundary Condition on the cut faces.  On solid elements (not shell elements) all that is required is add a Displacement of X=0 leaving Y and Z Free to make the Symmetry BC.

      All the contact in the model is Bonded contact, but some of that should be Frictional contact. The contact between the outside of the balloon and the outer cylinder must be Frictional.

      Four solids are used to make the Nylon bead on each edge of the balloon. It will be more efficient to combine those into a single solid for ease of meshing with good quality elements.


      The model uses Bonded contact to connect the nylon to the rubber. This slows down the computation. It is better to open the geometry in SpaceClaim, put the nylon body in the same part with the rubber body and use the Share button on the Prepare tab. That will create Shared Topology which will make the meshes share nodes where the two parts touch so no contact will be required.

      The rubber is much more flexible than the Inner Cylinder or the Outer Cylinder, so much more flexible that the metal parts are practically rigid. Change the metal part Behavior from Flexible to Rigid. This will eliminate all the mesh on the inside of the metal parts and only mesh the faces where contact is defined. This will speed up the computation. The Inner Cylinder makes almost no contact with the balloon, so that part can be suppressed entirely in the simulation and the two faces of the balloon that would have touched it can have a Displacement Boundary Condition.


      Use a 2 step solution. Step 1 is to inflate the balloon by ramping pressure up to 0.45 MPa, while holding the outer cylinder fixed. Step 2 is to move the outer cylinder axially while holding the pressure fixed. Use a Translational Joint with a Displacement Load. Probe the Joint Force as the upper cylinder moves to calculate the Air Spring stiffness.

      How far should the Joint move the outer cylinder?  Should it move up and down or just up?

      Under Analysis Settings, turn on Auto Time Stepping and allow the solver to select the needed Substep size by providing a range. I used 200 Initial, 50 Minimum and 50000 Maximum Substeps.

      In the figure below, the Axial (joint X-axis) joint Force at the end of inflation is 27884 N.

      The displacement was 100 mm down, so at Time = 1.1, that is 10 mm of travel. The spring rate is therefore the change in Force over the travel or (30044-27884)/10 = 216 N/mm for the half model. The full model will be double that, or a vertical stiffness of 432 N/mm.

      If you build this model with a Rigid Inner Cylinder, you will find that you can’t assign a pressure to the faces like you can when it is set to Flexible. This means that you have to calculate the force on the Inner Cylinder by dividing the pressure by the projected area of the Inner Cylinder. I drew a circle and filled it so I could measure the area as 0.0706 m^2. The pressure is 0.45 MPa so the vertical force is 31.8 kN, which is a full circle. The average Joint Force in the half model used to get the stiffness is 29.0 kN, double that to get the full model. Add 58.0 kN to 31.8 kN to get a total vertical load of 89.7 kN, which I plotted as the blue star below.

      Good luck!

    • Yun Wei Chuang
      Subscriber

      Hi Peter

      Much appreciate for your suggestion. It is truly useful to solve the model. 

      This model could be the as-molded shape but I will ask my teacher tomorrow on the class.

      You mentioned that the metal parts can be changed from Flexible to Rigid, but there are something turn to different I do not understand.

      Could you explain how you adjust the contact/target faces?

      The nylon bead and the steel steel wire I afraid they can not be contained together. The name "nylon tire cord" which is the important part for the air spring.

      Right now my idea is use 2 step to solve the model:

      step1: give the presure to 0.45 Mpa and find out the displacement ( from that point x=0) => F=KX

      step2: add force(finally force should be 130000 N) to calculate the stiffness Kz(k=f/x)

      THX

      Wayne

    • peteroznewman
      Subscriber

      Hello Wayne,

      Here is a link to the archive of my model: https://jmp.sh/JAv0DyAC

      When you change a Flexible part to Rigid, you can’t apply a Pressure load. Reread my description above where I explain that the force caused by the missing pressure is calculated by hand.

      When you change a Flexible part to Rigid, the Contact must have the Rigid part on the Target side of the Contact definition. Right click on the contact and select the Flip item in the popup.

      In the 1020 model archive, I missed that the circular part was Steel. You will need to recreate the Steel wire if you want to use my model. Use a smaller diameter to allow the nylon to have space to mesh around it.

      The way I did my model, holding the Outer Cylinder fixed while the Balloon inflates is more efficient from a solution elapsed time point of view. Raising the Outer Cylinder using a Displacement Joint Load in step 2 is also more efficient for solution elapsed time. You will find it takes longer to solve if you allow the Outer Cylinder to rise while the inflation takes place, then push it back down.

      Stiffness is the derivative of the Force-Displacement curve.

Viewing 9 reply threads
  • You must be logged in to reply to this topic.