contact FEA

[martin99]

Hi all,
I’m having some problems getting a spherical ball and socket to converge using linear contact and was hoping somebody had some practical advice on contact models. The model starts by converging nicely and looks like it will converge by about the 6th iteration but unfortunately it just seems to bump along with a couple of contacts that won’t converge. I’m currently using linear analysis due to the small displacements but I’m starting to think it’s non linear due to some bending of the ball component causing rotation and hence the contact elements no longer being normal to each other. When run as non-linear it also looks to converge then bumps along with a couple of un-converged elements.

Also after specific advice and some explanation on setting penalty factors and how they influence convergence and accuracy. I want to know why (according to ideas help), ‘the softer the target surface, the smaller the penalty number and why ‘large penalty numbers can speed up convergence’. It would be a start to know what ideas means by ‘soft’, ‘small’ and ‘large’.

When I have managed to get results for ball and cup problems the results always seem to be an order of magnitude different from mechanical testing!! The problems in getting the contact to converge means I haven’t been able to undertake an accuracy checks on the convergence of the mesh though.

Any comments on contact (both linear and non-linear) with ideas will be gratefully received. There is an image of the mesh at

http://www.martinmathias.com/contact

Many thanks in advance

Martin

 

[fsi]

Have u tried the surface dependency feature? This will ensure the same mesh on both contact surfaces and element normals will meet.

 

[martin99]

Many thanks for suggestion, but I’m not sure how much it will help on solving. If I have it wrong maybe you could let me know.

Here is my understanding:
Using surface dependency will only ensure the contacts are normal on the first iteration. On a linear run the contacts are not ‘re-searched’ between iterations so any displacement that is not normal to the contact pair will still make the pair ‘skew’ and therefore less accurate e.g. small rotation of the cup.
With a non-linear run dependency would again help convergence of the first iteration but the contact pairs are searched for between iterations therefore keeping the pairs normal to the load.
As the solution appears to converge well at the beginning I’m not sure how beneficial surface dependency would be on solving. Saying that my two meshes are quite dissimilar and making them the same can only be a good thing. Unfortunately I have never had much luck creating surface dependency, particularly with spherical surfaces. I will attempt it today though.

Many thanks

Martin

 

[fsi]

I have had cylindrical contact problems that did not converge, but when I tried the surface dependency it did converge. But spherical surfaces could be different than cylindrical sufaces, I have not tried that. Is there an initial gap between the two srfaces?

 

[martin99]

I ran a linear run last night with dependent contact surfaces (seemed very easy to get dependant surfaces this time). Whilst the solution didn't converge the results were in the right order of magnitude when compared to mechanical test results, also the cholesky pivots looked better, so i'm a bit more optimistic.

There is a very small separation of the contact surfaces of 0.05mm to start with. I'm still a bit in the dark with penalty factors could these be why it doesn’t converge and I would really like to understand them.
Ideas help states that low friction penalty factor, i presume this is the 'tangent' value in the options, should be low for sliding or sticking contacts....which they are. Also normal penalty factors should be low for soft materials......which it is not (ceramic).

We have a nice dual-processor workstation doing nothing this weekend in the office I might try a non-linear run on it. I thought if doesn’t converge on a linear run it is un likely to on a non-linear (unless the displacements are large), any thoughts? Many thanks again.

03:41:08 (CP 0.13 8310.18) Number of contact status changes: 3
03:41:08 (CP 0.00 8310.18) Number of inactive contacts: 3398
03:41:08 (CP 0.01 8310.19) Number of active open contactS: 0
03:41:08 (CP 0.00 8310.19) Number of sticking contacts: 0
03:41:08 (CP 0.02 8310.20) Number of sliding contacts: 124

 

[toothroot]

Hi Martin,

Although I'm not an expert in contact analysis, I'd like to ttry to help you. You're currently using tetrahedron element, I guess parabolic ones (tetra8). As far as I remember, parabolic tetrahedra are in general not very well suited for contact problems, because the edge nodes don't carry any (or hardly any) contact forces. I would recommend you to mesh your part with lineas hexaeder elements (mapped mesing), although that might give you some work.
You also might want to look at other FE programme systems, especially at ABAQUS which is said to be the top player in the contact field (as far as I've heard). I-DEAS has strong limitations; as soon as simulations become too complex (and contact problems are definitely complex), the solver is not able to give reasonable results.

Regards,
Daniel

 

[martin99]

Many thanks Daniel.

I am indeed using parabolic tets, I'll map mesh one contact surface and and apply surface dependancy for the other using linear tets for both. Is there any problems I should be aware of mixing linear and parabolic elements?

Cheers

Martin

PS Who said automatic mesh generation would make FEA easy!!!

 

[fsi]

I think Daniel is asking you to mesh your entire part with linear hexahedral elements (mapped meshing). I agree with him if your part is not complex and this can be done.

 

[toothroot]

Hi Martin,

yes I wanted to suggest that you mesh the entire part with linear hexaeders.
After looking at the picture of the model, I would also suggest that you try to simplify your model in order to make it smaller (less dof's). Depending on the load case, you could only model a quarter of the model, or even a small wedge (5° or so). As well, try to reduce the size of the orange or golden orange part. By that you should end up with a model that you can solve within a few hours instead within a weekend. Once you have a converged solution you can then step by step enhance the model again.

Regards,
Daniel

 

[martin99]

Many thanks that is very helpful.

I just did a very course mesh with linear tets and it solved in about 3mins. I forgot the speed on of linear tets although insuring accuracy is the thing now. I haven’t really used linear tets for structural analysis before. I’m thinking it’s ok as long as the mesh is properly converged is that correct?.

Do I just need to converge the mesh in a normal why i.e. make sure there aren’t any steep gradients on a few elements and stop refining the mesh when the stress results change is less than 5% per refinement?

I wasn’t going to map mesh, just use surface dependency on the contact area and add free locals if and where necessary. I think map meshing would prohibitively increase the time to converge the mesh, and if my last paragraph is correct, get accurate results.

Unfortunately I can’t simplify the model any further by symmetry due to lack of symmetry or even anti-symmetry of the boundary conditions.

Many thanks again, comments and suggestions still gratefully received.

Martin

 

[martin99]

oops, just relised you guys said linear hexahedral. I'll have to look into this, sorry for not reading your replies properly.

Martin