Register to reply

Difficulty in analyzing automotive tire in workbench

by amanmahajan
Tags: #ansys, #fea, #tire, #workbench
Share this thread:
AlephZero
#19
Nov12-12, 01:48 PM
Engineering
Sci Advisor
HW Helper
Thanks
P: 6,957
Quote Quote by amanmahajan View Post
For now I am just modeling it as a single rubber entity. I have not yet considered the steel reinforcements that go into it.
Quote Quote by amanmahajan View Post
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
#20
Nov12-12, 01:59 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,242
Quote Quote by AlephZero View Post
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.
amanmahajan
#21
Nov14-12, 02:00 PM
P: 17
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.
amanmahajan
#22
Nov21-12, 10:57 AM
P: 17
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
#23
Nov21-12, 12:44 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,242
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:

Quote Quote by Mech_Engineer View Post
  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.
http://www.physicsforums.com/showthread.php?t=433240&
amanmahajan
#24
Nov21-12, 01:37 PM
P: 17
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
#25
Nov21-12, 02:15 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,242
Try applying the load steps in reverse- deform the tire first and then apply the internal pressure.
Chestermiller
#26
Nov21-12, 07:19 PM
Sci Advisor
HW Helper
Thanks
PF Gold
Chestermiller's Avatar
P: 5,060
What you are doing is not even close to a realistic analysis of an automobile tire under inflation loading or under contact loading. In a real tire, the tire cords carry most of the load, and the rubber is there just to glue the cord plies together and to prevent the air from escaping from between the cords. Have you looked into the literature on structural analysis of automobile tires, such as Tire Science and Technology. Early analyses of tires used membrane models which accounted for the effects of the tire cords. Later analyses used bending models, and finally, more recent models used detailed finite element. All these took into account the composite nature of the structure.
amanmahajan
#27
Dec1-12, 12:10 PM
P: 17
Hello Mech_Engineer,

I was able to sort out the problem related to the surface and tire contact.
My next step in the analysis is to check the stresses induced in the tire as it rolls on the ground. Can you advise me some steps to get started with that.

Thanks for all your help
Mech_Engineer
#28
Dec1-12, 12:51 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,242
My feeling is you're better off making a more realistic model of the tire first, including the belts. Doing all this work to get the model working will have to be done again otherwise.
amanmahajan
#29
Dec1-12, 12:58 PM
P: 17
Hello Mech_Engineer,

My advisor first wants me to get a steady state rolling analysis to work and then I will add the reinforcements to the rubber.

That's why I asked for your help to get started on the analysis for rolling.

Thanks
Aman
amanmahajan
#30
Dec10-12, 12:05 PM
P: 17
Hello Mech_engineer,

I have successfully modeled the tire to a close approximation of the real scenario. Can you now please guide me through the process of steps needed to analyze its rolling on a surface to see the stress variation

Thanks
Aman
Mech_Engineer
#31
Dec10-12, 06:10 PM
Sci Advisor
PF Gold
Mech_Engineer's Avatar
P: 2,242
Well it depends on what conditions you want to analyze it under. You need to consider things like angular speed (centripetal acceleration), applied torque, and load it's supporting. You're going to have to decide how you want to approximate ground moving by as well.


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