I was working on the same thing this AM. I can not get the shrink fit to work in an NL analysis - well I got results once and they looked non sensical but then it would not run again with the same settings. I actually wan thte preload condition as a shrink fit and then do a sliding contact analysis with friction after that. I have tried all the various contact options, surface to surface and node to surface with varying mesh densities on the contact patch and no joy.
The other option, which I have not done recently but in the past has not worked either is to apply a pressure or force to contract the the ID so that it is smaller than the OD and then relax the force back to zero and have the contact get etablished that way and then move on to the next step.
I tested the model in a static study first to see if the analysis would run as linear contact problem. It did but the results for my case did not look very good. My case is essentially a stiff cylinder covered by a low stiffness material press fit into a stiff outer cylinder. The cover on the inner piece has s stiffness of about 25000psi in the linear analysis and is actually a hyper elastice inthe NL analysis. The other peoice are linear at about 350 ksi in stiffness. The about of interference is about .005"
Pretty frustrating really.
I am trying the press fit analysis with nonlinear analysis and I am able to finish 61% of the displacement out of 100% but then the analysis stops giving some error messages like ETAN>EX/100, Tolerance < 0.5< 0.0 and also PCGLSS0139 error in solver.
I tried refine the mesh but didn't work out and I know it is happening because of negative pivot error ( singularity error) . I have solved these problems in Ansys and it is pretty fast. Solid works simulations don't have control on penetration tolerance, normal contact force and etc.
I am trying out this and will see to that it gets solved and also I will try solving using shrink fit contact and find out difference.
Akash A V
Good luck. You are going to need it. It would be nice if whatever you find was "robust". However, I am not optomistic and won't be holding my breath. Good on you for giving it a whirl though.
ETAN>EX/100 sounds like a problem with the non-linear material part of the analysis. Are you using material curves or ISO or Kinematic hardening rules?
Good to see all your reply. Thanks alot for all your help and kindness.
I have solved the problem with complete nonlinearity. I have nonlinear frictional contact, large displacement and large strain ON.
The press fit analysis works completely. As per the Paul Kellner, the material tangent modulus was not proper to model bilinear isotropic hardening. No the analysis runs with out any error messages and solves properly.
Now I see the radial displacement of outer body and also the plastic strain.
Please find the analysis stress plot for the final load. So still the typical analysis procedure works, if we still dont have shrink fit contact.
Way to go! Any chance I can get that model? Probably not and I get why.
Could you answer a couple questions and/or confrim some settings then:
- The analysis sequence was: press fit followed by the slide for full the insertion? Ther press fit has no time curve so it happens in the first step, was the slide curve just 0 to 1 or was it different than that? If so what was it?
- The contact definition was surface to surface or surface to node?
- Coeff of friction was?
- Paul or Akash, Why would it matter what the hardening rule is as there does not seem to be any unloading present?
- What was the max strain? and what was Ex and Etan if you would or what materials are involved?
- It doesn't look like the large strain option would be needed, does it solve without it on?
I dont think so i will able to give up the model and sorry for that, but i can give my answers to the above mentioned queries:
1) The load has to be ramped and not stepped, but since it is diplacement control, hence it is stepped loading. hence we need to apply very gradually. The load will vary from 0 to 1 with small step change. Care should be taken so that no step change cause high plastic strain increment. Also switch to automatic time step increment with initial step change to 0.001.
2) I have used surface to surface, as it is robust when dealing with penetartion problems,as it aids for better convergence.As here for every iteration it checks for penetration value and adjusts the stiffness of underlying elements
3) fricition co-efficient was 0.20 and any thing beyond 0.25 swithec it to unsymmetic matrix and solver. makes it difficult and time to converge
4) You are ture there is no unloading, but both these rules work in a different way.
5) maximum plastic strain was 0.010mm/mm, that is 1% dilation. the EX was 205e5MPa and Etan 665 MPa for hole and Etan 2416MPa for pin. The material are throug and case harden steel
6) Ya offcousre it solves with out large plastci strain, but it is always advisble to check with large stain On, as the metal plasticity is involved.
I have answered to best of my knowledge and you may not consider this as the best and may have better one.
Please correct me if I am wrong in any way. Will appreciate your feedback
Of course you can run your model adding complexity to the run each time.
1. No friction, no plasticity, displacement control
2. Friction, no plasticity, displacement control
3. Friction, no plasticity, riks control
4. Friction, plasticity, displacement control
And you can vary this with different solvers along the way. But #1 is the important first run. It will show the high stress areas. If you know where the high stresses are you can limit the elasto-plastic material solving to those areas which should help your run times.
Glad to see that you got your simulation to run. My one concern would be that the coefficient of friction at 0.2 is too low for steel on steel unless the parts are lubricated. Assuming your parts are not lubricated, then I would definitely follow Paul's advice and solve once with no friction to compare the results. If you can't get it to solve with a coefficient more like 0.4, then you can at least extrapolate from the two results to get a better idea of the "real" results.
This rather facinating thread reminds me to try the 2D solver when I upgrade. I havent had a chance to try the 2D solver in 2011 and 2012 yet. Does it run nonlinear and would switching off friction work?
In Cosmos/M the only limitation on PLANE2D elements is that they cannot handle Composite Failure criterion. The ability to do elastic/plastic analysis is a function of element formulation. Just what they carried over from Cosmos/M to Simulation I can't say but chances are you can. Cosmos/M has had this capability since MSDOS days.
Switching off friction should work as far as the solution goes.
And Jerry's comment about friction coeficient touches on the problem that goes along with all non-linear phenomenon like this: results are path dependent. So it is possible the OP wants to run a series of models varying the friction coefficient and perhaps loading variations to see what it's sensitivities are.