Axi-symmetric Contact Model does not converge after refining mesh

[coolFL]

Hello all,

I am solving one simple Axisymmetric model of ball resisting on disk. Contact is established between ball outer surface and disk top surface. Uniform pressure is applied at the top surface of the ball. I am getting contact pressure with reasonable accuracy but the problem is in determining exact contact dimensions. For this when I refine mesh of the model, then contact pressure start to diverge. Plus after certain refinement(of both Master and Slaves surfaces) Abaqus couldn't simulate the model. Does any body know how to tackle this issue of mesh refinement? I mean how to ensure that in contact analysis results converge after refining mesh of both master and slave surfaces. I have also attached .CAE file of model along with this message.
Any help in this matter will be appreciated,
Thank you in advance,

Sincerely,
Nikhil

 

[corus]

You may get better convergence if you apply a set displacement to the ball in the 1st step and then apply the load in the 2nd step.

 

[coolFL]

Hey, Thanks for the reply!
I tried your suggestion and I am facing following issues:
1) Convergence is slightly improved i.e. my model is converging even after slight mesh refinement. But beyond certain limit of mesh refinement model is again not converging. Model converges when there are around 20 elements along the slave contact edge. But it doesn't when number of elements are increased up to 50.
2)The two step approach gives slightly inaccurate results than the one step approach. Contact pressure values are more accurate for one step approach than the two step approach.
3)Contact pressure values are also very much sensitive to the magnitude of displacement that is given to the ball in 1st step. I tried various displacements but contact pressure values are not as accurate as the one step approach. So is there is any criterion for deciding the magnitude of displacement in the first step?
Any guidance on these issues will be appreciated,
I have attached the .cae file with results for different displacement magnitudes.

Thank you in advance,

Sincerely,
Nikhil

 

[corus]

The amount of displacement is irrelevant to the results of the 2nd step as the displacement is removed from the 2nd step. The displacement is there simply to provide contact reaction forces between the two bodies so that in the 2nd step you avoid equilibrium problems that may occur with one body being unrestrained. It may be that the problems you have are due to the rapid change in mesh density with the poor aspect ratio in the coarser mesh. I'd reconsider how you mesh the two bodies so that there is a more gradual transition from fine to coarse regions, perhaps using a bias in the element size along the edges away from the fine mesh region.

 

[coolFL]

Hey, Thanks for the information!
To verify the effect of rapid changes in mesh density, I reformed the analysis without any face and edge partitions on the two bodies. So in the current model, I have uniform mesh through out the two bodies and mesh density is also almost constant over the entire domain as no bias ratios were used. The observations for this model are as follows:
1) With very fine mesh refinement solution is still converging. So the original issue of convergence is resolved.
2) One very good thing about new model is that results for quadratic elements are more accurate than those for linear elements. In the original model it was other way around i.e. linear elements, with reduced integration option on, used to give more accurate answers. This is unusual as Hertz contact pressure decays quadratic-ally along the contact edge. Therefore we should expect quadratic elements to be more accurate. The only conclusion of this exercise is that partitioning faces/edges is not a good idea as it alters the results due to changes in mesh densities.
3)Most important issue: As in the original model, new model (without any face partitions, no bias ratios which means uniform mesh density) also shows that final answer (i.e. contact pressure) is still very much dependent on initial displacement given to the ball. If the displacement is of the order of 10^-6 then there are convergence issues. And the contact pressure slowly decreases as we increase initial displacement from 10^-6 to 0.01 mm. I still don't understand any reason for this behavior. As you mentioned, variation in mesh density is reduced in this model but the results are still dependent on initial displacement(even for model with very fine mesh). Any further guidance to resolve this issue would be appreciated.
I have attached .cae file of the new model. It is under 1000_without mesh partitions.
Thank you very much in advance,

Sincerely,
Nikhil