Asymmetry in symmetric contact problem

[erolsson]

Hi!

I have a problem with modelling contact between two axi-symmetric spheres in ABAQUS v 6.10. The spheres have the same radii and the same material

E = 455 GPa
yield stress = 50 MPa
Ideal plastic

I know that the material is "extreme" but the purpose with it is to simulate fully ideally plastic contact which has a theoretical solution. The solver doesn't give any errors or warnings but the solution becomes asymmetrical with respect to the contact plane as the contact grows. One sphere behaves much softer than the other after 400 increments (increment length 1E-4).

The mesh is fully symmetric and the contact pair (surface to surface) is defined twice with master-slave switched to ensure full symmetry.

Smaller increments and a denser mesh doesn't help
With a linear elastic material, no asymmetry exist and the solution matches the theoretical Hertz' solution.

I attach a zip file with a picture of the plastic strain where the asymmetry is shown and a file with my python script

Thanks for your help
Erik

 

[rstupplebeen]

To me it looks like the nodes become slightly misaligned. I believe that this is due to numerical noise. My guess is that it randomly goes one way or another.

I would suggest using X symmetry on the Y axis. I was just informed by someone at Abaqus that it is handled slightly different than if you simply constrain X and rotation around Z. Basically the solver knows that the elements on the symmetry plane are horizontal at X=0 not the arbitrary faceting of the mesh.

Why not model this with symmetry by having a rigid plane and only 1 sphere?

I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[rb1957]

i suspect it doesn't really like perfectly plastic material ... i'd give the material curve a small +ve slope after yield (rather than zero slope).

 

[corus]

The lower sphere appears to bulge as if the upper sphere is stiffer and pushes into the lower sphere. I doubt it's the mesh as they're both equal in size and should have the same stiffness (a coarse mesh will be slightly stiffer in practice). 400 increments seems to be a lot and it appears that the job never finished. With contact and plasticity you might be better using explicit rather than standard, as it works better with such gross non-linearity.

Tara

http://tinyurl.com/4ydjg7m

 

[mechfeeney]

I ran the job on my machine and got a symmetric results for stress. Look at different field output plots and observe that you have symmetric results. As for PEEQ, my guess is your mesh is not refined enough. Tighten it up and I bet you will get a symmetric plot. It appears as though I got slightly different values than you too.

 

[mechfeeney]

Here's the stress plot.

 

[erolsson]

Thank you everyone for your help!

rstupplebeen: The reason why I'm not modelling one sphere and a rigid plane is that when this "simple" case works, I will start with spheres of different radii and material.

I put convert SDI on and it helped up to a time step of ~8E-2.

mechfeeney: Thanks for running my file! The asymmetry shown in your first post will get worse for larger indentation depths which I unfortunately will have to analyse. The stress plot looks symmetric at a time step 0.1 but will not be symmetric at 0.2 or 0.5

I will try now with a power-law hardening material and see if the problem remains

Thanks
Erik

 

[corus]

I ran the python script file, with a only a slight modification to the step definition so that the job wasn't limited to a time step of 1e-4. The results look fine to me for PEEQ using 6.11.1. See picture (results mirrored).

Tara

http://tinyurl.com/4ydjg7m

 

[mechfeeney]

corus, isn't that still at 0.1s?

 

[corus]

Yes, as it was in the python script. I'll edit the file and post results for a longer time step later.

Tara

http://tinyurl.com/4ydjg7m

 

[mechfeeney]

Yeah I made that mistake too. In all fairness the fact that it was relatively symmetric at .1s and not at .4s was something that should have been stated at the beginning of the thread : ]

 

[erolsson]

mechfeeney: Of course, I apologize for that!

I'm now trying with stricter convergence criteria to see if that reduces the problem.

My hope is to simulate an indentation depth that is so large as 5 % of the particle radius

/Erik

 

[corus]

I ran the job up to 1 second and see the asymmetry in the results. As far as I can see there are no errors in the inp file either and the only warning in the dat file refers to the defined contact controls not being needed.

Up to about 0.1 seconds the results are symmetric and after that they differ. The only explanation I can think of is that the asymmetry comes about because the nodes mismatch after that time, and the mismatch increases over time. Strangely at 0.1 seconds you can see that one contact surface penetrates the other at one point, even though double contact surfaces have been defined which should prevent this.

I'm not sure if the problem isn't due to the units being used, so that the element size is close to absolute tolerances Abaqus may use internally. If it's possible use more 'whole' numbers for the geometry. I'd also try using the automatic tolerances for the contact controls, which tends to smooth out contact.

Tara

http://tinyurl.com/4ydjg7m

 

[erolsson]

Dear all

The problem is know solved by changing to hybrid elements (CAX4H) and Node-to-Surface contact which I find a little bit strange because I thought that Surface-to-Surface contact was superior in almost all cases.

The problem is know symmetric (to the last digit) for indentation depth of 5 % - 10 % of the particle radius

Thank you
/Erik