Asymmetry in symmetric contact problem
Asymmetry in symmetric contact problem
(OP)
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
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





RE: Asymmetry in symmetric contact problem
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/
RE: Asymmetry in symmetric contact problem
RE: Asymmetry in symmetric contact problem
Tara
http://tinyurl.com/4ydjg7m
RE: Asymmetry in symmetric contact problem
RE: Asymmetry in symmetric contact problem
RE: Asymmetry in symmetric contact problem
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
RE: Asymmetry in symmetric contact problem
Tara
http://tinyurl.com/4ydjg7m
RE: Asymmetry in symmetric contact problem
RE: Asymmetry in symmetric contact problem
Tara
http://tinyurl.com/4ydjg7m
RE: Asymmetry in symmetric contact problem
RE: Asymmetry in symmetric contact problem
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
RE: Asymmetry in symmetric contact problem
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
RE: Asymmetry in symmetric contact problem
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