Difficulty in analyzing automotive tire in workbench

amanmahajan

Hi,
I am trying to analyze the effects of pressure on the automotive t=ire by modeling and simulating the same in ANSYS workbench. However, I am having trouble applying material conditions to the model.
I wish to use mooney rivlin material but when I apply that based on the guidance given by the following link, my solution does not converge.

video link: http://www.youtube.com/watch?v=Kt-AbUrxV1g

My boundary conditions are fine because if I use a material such as steel, I get a solution.

Kindly help me and let me know where I could go wrong.

xxChrisxx

The material behaves non linearly and you are using a linear solver.

amanmahajan

Chris,
Can you please tell me what changes to make in order to run the analysis.
Thanks

Mech_Engineer

You need to use a non-linear solver (selecting "program controlled" is probably fine too), and you need to split a largely nonlinear problem into a lot of substeps. Depending on the amount of deflection you're seeing, it could be on the order of hundreds of substeps.

amanmahajan

Mech_Engineer,

I used program controlled but that failed
So I used substeps as
Initial - 100
Minimum - 10
Maximum - 1000

Using this too the solver ran for a long time but it didn't solve.

I increased the newton raphson residuals to 4 to see where the force convergence was a problem and it appeared to be along the sidewall.
I increased the no. of elements by refining the mesh but that too has not solved the problem.

Is there anything else that can possibly be wrong with the solution?

Thanks

amanmahajan

Following are the error messages that I obtained:
substeps:
initial: 20
minimum: 10
maximum: 100

Attached Thumbnails

     

amanmahajan

two more errors continued.

Attached Thumbnails

   

Mech_Engineer

• What does the force convergence chart look like, was it slowly converging or bouncing all over the place?
• Are you sure that your model is fully constrained? Does the deflection look something like you're expecting or is it mainly solid body movement?
• Are you applying a contact condition on the bottom of the tire? What properties are you applying to that boundary?

amanmahajan

Mech_Engineer,

The convergence curve begins from below, oscillates about the main line. I do get points in the run where there is convergence but the last two or three points don't converge leading to no solution.

The boundary conditions are alright because if I apply steel as the material to the same model, I get results without any problems.

I am currently analyzing the stresses developed in the tire only due to the inflation pressure. So there are no contact conditions needed to be developed.

Please help.
Thanks for your reply once again!

Mech_Engineer

It sounds to me like the model isn't converging because you don't have enough substeps. You should consider increasing the number of substeps, and applying your pressure gradually through load steps.

Ideally, the force convergence graph should start above the line and converge to below the goal line. If it oscillates about the goal line a lot I'm thinking it means the perturbed system is oscillating; a gradually applied and solved-for load may help with this.

amanmahajan

Mech_Engineer

Thank you for your reply. I will try what you suggested and get back to you after that.

amanmahajan

Mech_Engineer,

I tried the simulation changes that you had recommended but I am still facing the same problem.

Mech_Engineer

I think you're going to have to try some simplification and see what it takes to get it to converge, either through a simpler geometry and/or simpler material model. Once you're able to get a solution, you can slowly add complexity and see at what point the model is no longer converging. My guess is the pressure load needs to be applied slowly with load steps; how much pressure are you applying? Have you tried a lower pressure to see at what point you can get a solution?

amanmahajan

I am applying a pressure of 0.7 Mpa.
No, I have not tried to apply a lower value of pressure on the tire yet to see if that works ok.
I will be doing that now to see if I get some convergence.
Thanks

Mech_Engineer

Try applying something much lower for a start and see how it goes. A pressure of 0.07 MPa might be a good starting point, and could provide you with the structure of load-stepping up from there.

It seems possible your tire is not able to hold 0.7 MPa and is failing to converge because it is structurally failing. A lower starting point might help you visualize this.

amanmahajan

That makes sense.
However, the pressure that I applied is the recommended maximum pressure for the tire. But I see what you mean. I'll decrease the load.

Mech_Engineer

When you say you're modeling a tire, do you mean the steel belts and everything? Tires are a pretty complex composite design of rubbers, polymer bands, and layered steel mesh belts; it seems to me they would be a complex analytical challenge.