Difficulty in analyzing automotive tire in workbench


by amanmahajan
Tags: #ansys, #fea, #tire, #workbench
amanmahajan
amanmahajan is offline
#1
Nov7-12, 12:52 PM
P: 17
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.
Phys.Org News Partner Science news on Phys.org
SensaBubble: It's a bubble, but not as we know it (w/ video)
The hemihelix: Scientists discover a new shape using rubber bands (w/ video)
Microbes provide insights into evolution of human language
xxChrisxx
xxChrisxx is offline
#2
Nov8-12, 02:57 AM
P: 2,032
The material behaves non linearly and you are using a linear solver.
amanmahajan
amanmahajan is offline
#3
Nov8-12, 08:25 AM
P: 17
Chris,
Can you please tell me what changes to make in order to run the analysis.
Thanks

Mech_Engineer
Mech_Engineer is offline
#4
Nov8-12, 09:31 AM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,234

Difficulty in analyzing automotive tire in workbench


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
amanmahajan is offline
#5
Nov8-12, 10:35 AM
P: 17
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
amanmahajan is offline
#6
Nov8-12, 10:44 AM
P: 17
Following are the error messages that I obtained:
substeps:
initial: 20
minimum: 10
maximum: 100
Attached Thumbnails
error1.jpg   error2.jpg   error3.jpg  
amanmahajan
amanmahajan is offline
#7
Nov8-12, 10:45 AM
P: 17
two more errors continued.
Attached Thumbnails
error4.jpg   error5.jpg  
Mech_Engineer
Mech_Engineer is offline
#8
Nov8-12, 12:41 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,234
  • 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
amanmahajan is offline
#9
Nov8-12, 02:46 PM
P: 17
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
Mech_Engineer is offline
#10
Nov8-12, 04:24 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,234
Quote Quote by amanmahajan View Post
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.
amanmahajan
amanmahajan is offline
#11
Nov8-12, 11:08 PM
P: 17
Mech_Engineer

Thank you for your reply. I will try what you suggested and get back to you after that.
amanmahajan
amanmahajan is offline
#12
Nov12-12, 10:19 AM
P: 17
Mech_Engineer,

I tried the simulation changes that you had recommended but I am still facing the same problem.
Mech_Engineer
Mech_Engineer is offline
#13
Nov12-12, 11:41 AM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,234
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
amanmahajan is offline
#14
Nov12-12, 11:43 AM
P: 17
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
Mech_Engineer is offline
#15
Nov12-12, 11:59 AM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,234
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
amanmahajan is offline
#16
Nov12-12, 12:29 PM
P: 17
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
Mech_Engineer is offline
#17
Nov12-12, 01:11 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,234
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.
amanmahajan
amanmahajan is offline
#18
Nov12-12, 01:14 PM
P: 17
For now I am just modeling it as a single rubber entity. I have not yet considered the steel reinforcements that go into it.


Register to reply

Related Discussions
Comparing pressure of air in a tire installed in a car & a free tire General Physics 3
Workbench materials Mechanical Engineering 0
Automotive/Truck Tire Pressure Vs. Load Classical Physics 6
Find the radius of a car tire, given the mass of wedged stone & tire rotation in m/s Introductory Physics Homework 4