Difficulty in analyzing automotive tire in workbench

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:
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.
 
Last edited by a moderator:
2,014
85
The material behaves non linearly and you are using a linear solver.
 
Chris,
Can you please tell me what changes to make in order to run the analysis.
Thanks
 

Mech_Engineer

Science Advisor
Gold Member
2,570
169
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.
 
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
 
Following are the error messages that I obtained:
substeps:
initial: 20
minimum: 10
maximum: 100
 

Attachments

Mech_Engineer

Science Advisor
Gold Member
2,570
169
  • 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?
 
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

Science Advisor
Gold Member
2,570
169
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.
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.
 
Mech_Engineer

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

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

Mech_Engineer

Science Advisor
Gold Member
2,570
169
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?
 
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

Science Advisor
Gold Member
2,570
169
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.
 
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

Science Advisor
Gold Member
2,570
169
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.
 
For now I am just modeling it as a single rubber entity. I have not yet considered the steel reinforcements that go into it.
 

AlephZero

Science Advisor
Homework Helper
6,953
291
For now I am just modeling it as a single rubber entity. I have not yet considered the steel reinforcements that go into it.
However, the pressure that I applied is the recommended maximum pressure for the tire.
The "recmmmended maximum pressure" will be for the real tire including the steel reinforcements, not for a rubber ring with no reinforcement.
 

Mech_Engineer

Science Advisor
Gold Member
2,570
169
The "recmmmended maximum pressure" will be for the real tire including the steel reinforcements, not for a rubber ring with no reinforcement.
Exactly what I was getting at. The model isn't converging because just rubber can't hold that much pressure. I'm guessing your modeling efforts will start to converge when you apply less pressure, but the deformations won't really match those of a "real" reinforced tire.
 
AlephZero & Mech_Engineer,

I didn't think of it.
I found my mistake. When I reduced the pressure significantly to 0.06 psi, The solver was able to converge.
Thanks for all your help. I will go ahead into my analysis now and will post any further problems that I face.

Thanks again.
 
I am now trying to analyze the same tire by applying contact conditions between the tire and a surface below it. The surface has been modeled as a plate underneath the tire and I have specified frictionless contact.
I try to press the tire against the surface, keeping the inner pressure as 0.05Pa but the results do not converge. Can someone please advise me what could be the error.

Thanks
Aman
 

Mech_Engineer

Science Advisor
Gold Member
2,570
169
Take a close look at all of the things we've talked to you about already, but in addition make sure you using all of the tips I listed here:

  1. Pay Close attention to your mesh density in the sheet metal being bent, as well as in the contact conditions that are moving it. The mesh should be of similar size on both sides of the contact, you can use a "contact condition mesh refinement" to make sure this happens.
  2. Make sure you use an "Augmented Lagrange" formulation for the contacts between the sheet metal and press. This formulation will work best with sliding conditions.
  3. As a start, make the contact condition between the sheet metal and press frictionless. Once you get it to converge, then you can think about considering friction.
  4. Make sure your contact condition forces update every substep, and split your problem into MANY substeps (on the order of 100).
  5. Make sure you have accurate material data for your sheet metal, especially into the plastic deformation region which you'll be probing specifically.
  6. Remove the "frictionless supports" which are nonlinear boundary conditions that I suspect will cause you undue grief, and replace them with fixed displacement conditions (0 displacement in axis perpendicular to surface).

That's a good start anyway... I'm not sure of your limitations using ANSYS Academic (the mesh is limited to what, 10K nodes or something?), but hopefully this will start getting you in the ballpark.
https://www.physicsforums.com/showthread.php?t=433240&
 
Mech_Engineer,

Thanks for your reply.
Here is the problem, The sheet below is simulated as a road surface. If I remove the internal pressure on the tire and displace the sheet upward by 1 mm, the solution converges. This is the case where the sheet is a flexible steel.

However, if I consider the sheet with rigid stiffness behavior in material properties and run the same simulation, the result won't converge.

Additionally, keeping everything the same as the first case, if I apply internal pressure to the tire model and then displace the sheet upward, the solution doesn't converge.

I tried the things you asked me to but I still have the same issues.

Kindly help
 

Mech_Engineer

Science Advisor
Gold Member
2,570
169
Try applying the load steps in reverse- deform the tire first and then apply the internal pressure.
 

Related Threads for: Difficulty in analyzing automotive tire in workbench

Replies
1
Views
3K
Replies
1
Views
978
  • Posted
Replies
3
Views
943
  • Posted
Replies
7
Views
14K
  • Posted
Replies
1
Views
5K
Replies
12
Views
21K
Replies
2
Views
2K
Replies
2
Views
5K

Physics Forums Values

We Value Quality
• Topics based on mainstream science
• Proper English grammar and spelling
We Value Civility
• Positive and compassionate attitudes
• Patience while debating
We Value Productivity
• Disciplined to remain on-topic
• Recognition of own weaknesses
• Solo and co-op problem solving

Hot Threads

Top