contact problem of adding load on a tire model to see its deformatiom

[jcfhh]

Hi all,

I am trying to do the simulation of lying a tire model on the ground horizontally and adding load on its sidewall to see its deformation.
I have already had my 2D tire model and it runs well. I think there is something wrong in my 3D input files since the msg file keep showing the error as:

CONTACT PAIR (SIDEWALL-DOWN,SROAD_2) NODE 55760 IS OVERCLOSED BY 14.0065
WHICH IS TOO SEVERE.
CONTACT PAIR (SIDEWALL-DOWN,SROAD_2) NODE 57135 IS OVERCLOSED BY 8.00135
WHICH IS TOO SEVERE.
CONTACT PAIR (SIDEWALL-DOWN,SROAD_2) NODE 57252 IS OVERCLOSED BY 8.94135
WHICH IS TOO SEVERE.

***ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT

Therefore I upload the 2D tire input and 3D input files to the link shown below.
Link
Could anyone please tell me how to solve this problem?
Thank you very much.

P.S. The tire model is a 2D file and then I use SYMMETRIC MODEL GENERATION to make it 3D through abauqs command windows. Hope this information is helpful to make you clear about my case.

Best Regards,
JAY

 

[Mustaine3]

Check the normal of the rigid road 2. You should use the negative side of that face for contact.

And don't forget to add some boundary conditions for that rigid.

 

[jcfhh]

Dear Mustaine3,

I have checked the normal of the road2 and I found that the direction of the normal is in wrong direction!
Could you please tell me how to change the direction of the normal in input file? Or is there any other solution to deal with this situation?
Thank you very much.

Regards,
Jay

 

[Mustaine3]

The surface that is used for contact is created with *Surface. Now look into the Keyword Reference Manual regarding the meaning of the dataline and you'll easily find the way to change the contact direction.

 

[jcfhh]

Hi Mustaine3,

You mentioned that I should use the negative side of that face for contact. Does it mean I hsould change the SPOS to SNEG? I tired it but it did not work.
The road2 has become sliding after this.
I also looked into the the meaning of the data line in the section of *Surface in Keyword Reference Manual and I cannot find anything related to change the contact direction.
I am so sorry but I am really stuck at situation for months. Could you please explain more specifically how I can find those information in the abaqus documentation?
Thank you very much.

Best Regards,
Jay

 

[Mustaine3]

I also mentioned that you should check the boundary conditions on your rigids.

When I tell you the solution, then you're not learning how to use the manuals. The next time you have a problem, you can't help yourself and have to ask others again.

 

[jcfhh]

Hi Mustaine3,

Thank you for your reply. I tried to add some boundary condition for the rigid road 2. And now the overclosured problem is solved. The tire is supposed to buckle when the load is applied on the road. However, the tire did not buckle and it became sliding this time. Therefore I upload the my new 3D input files to the link shown below:
Link
Could you please have a look and give me some comment if you are free? Thank you very much.

And also, the problem of the normal's direction has not been solved actually. My project adviser and I really looked into the the Keyword Reference Manual again but we really could not find the solution to change the direction of road2's normal. I am not sure if it is the reason why the tire did not buckle. I know you want me to solve it by myself but I really running out of time. Like I said I was stuck at this situation for months and my project deadline is in 2 weeks, I will not get my degree if I cannot finish this stimulation. Therefore, could you please give me some more advice on how to find those information? I would be very grateful. Thanks again.

Best Regards,
JAY

 

[jcfhh]

Hi Mustaine3,

Not sure if you have seen my reply yet. Therefore I reply again to hope you can see it and give me some advice.

Thank you very much.

Best Regards,
JAY

 

[Mustaine3]

Your load acts in the wrong direction and you BC are still not correct. You should fix all DOF beside the one with the load.
After repairing this the job runs to completion.

I also recommend to add some small amount of friction, otherwise the tire can slip without limits between the rigids.

 

[jcfhh]

Hi Mustaine3,

Really thanks for your reply. I have changed the load directions and the BC for the top rigid road and also added some friction the hold the tire.

The analysis is completed now. In the ODB file,I can see the tire deformed now, however, the there is no any pressure changed in tire. I think there is something wrong in my input file.

Could you please have a look on my input file if you have time?
Link

And also I have no idea how to fix the DOF problem since I am very new to abaqus. Could you please give me some advice on this?
Sorry for bothering you so long and thank you so much for being so helpful.

Best Regards,
JAY

 

[Mustaine3]

What pressure? In the 3D model is no pressure defined.

And what do mean with "DOF problem"? The BC seem to be ok.

 

[jcfhh]

Hi Mustaine3,

Thanks for your replying. I mean if the road is moving towards the tire, the tire would have some pressure changes and it would eventually buckle at a critical load and this is the main aim of my simulation.
The tire should change to barrel shape but instead it seemed the tire only became squeezed. I also tried to apply more load on the tire to see if it would buckle. However, when more load was applied ( let's say -10000N), the penetration error appeared and the analysis could not be completed. Do you think what the reason about this situation is?

About the DOF problem, when the analysis was completed. there are some warming messages appeared, It is shown below:

***WARNING: SOLVER PROBLEM. NUMERICAL SINGULARITY WHEN PROCESSING NODE 121
D.O.F. 1 RATIO = 149.166E+09

***WARNING: THERE ARE 2 UNCONNECTED REGIONS IN THE MODEL.

***WARNING: THE SYSTEM MATRIX HAS 1 NEGATIVE EIGENVALUES.

NEGATIVE EIGENVALUES MEAN THAT THE SYSTEM MATRIX IS NOT
POSITIVE DEFINITE:
FOR EXAMPLE, A BIFURCATION (BUCKLING) LOAD MAY HAVE BEEN EXCEEDED.

Do you think these warnings are the reason of my situation?

Thanks for taking the time out of your schedule to help me with my project.

Best Regards,
JAY

 

[Mustaine3]

How can you expect to get some behavior coming from an internal pressure without applying such a pressure?