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!