check the termination scheme - alot times they stop because you told it too without realizing it. Check the .out file for why it terminated if not obvious. Material properties not that big a deal as far as completion goes - not realistic sure. Hyperelastic materials are another story - the materail model data needs to be good. Tangent modulys is just a simple approximation of a stress strain curve using two lines, 30 msi & ~400ksi for mild steel as an example. Hardening factor is only on concerne if you are loading unloading and then loading again - capturing work hardening effects.
NL contact is not SWX simulation best game. Tet 10's are probelmatic from a numerical point of view. The contact formulation is a long way form state of the art. Getting htem started is very tricky - add some stiffness (weak springs) to any part where it is only restrained by the contact. Add small gaps to avoid coincident surfaces that are in contact (unless node to node is used) - may have to add artificial stiffnesses - keep them balanced as well. Constant time steps and uniform element sizes also good ideas if you get it going. You don't want a time step that yields a displacement much greater than half and element length. High aspect ratio's in a contact patch best avoided.
Hope that helps and Good luck.
Contact is by far the toughest non-linearity
Large displacement would be next (can be very tricky if things are crumpling as it usually involves self contact)
Material non -linearity - easy if metals and things that are stiff - incompressibles are trickier.
Thanks a lot for your very informative input. It helped a lot.
I blamed the wrong thing - material model. Right now, I can get non-linear going with whatever material model on COMponent. But not on assembly. It must be contact.
But I am still puzzled, because I am nonlinearly simulating an exactly model, which I can solve with static simulation without any issue. I took a look at .OUT file per your advice and the last paragraph says:
The automatic step adjustments exceeded 5 times
Contact/Gap algorithm is not converging; This is mainly caused
by singularity of stiffness matrix due to other nonlinearities
You may try to use the <restart> option
T O T A L R U N T I M E (Sec) . . . . . . . . . . = 7043
Reason I want to use nonlinear because we have to consider stress goes above yield point, but I can not get contact settled the same way as static (linear) simulation! Still looking ideas! Already shoot an email to our technical support. I had experience with Abaqus before, nonlinear. Didn't have this problem at all.
By the way I have a better idea about coincident contact that you don't want, which is to either supress or delete the global contact. It assumes a bonded contact if two parts are originally in contact and no manual contact is input.
Thanks a lot again,
I take it this at step 1?
Well this is the tricky bit and the contact in the static study is much more robust (ie it works better with a lot less experimental actions trying to get it to work) that what is in the NL solution.
here are a couple things:
0) Increase the number of step adjustment to 10 - it may just take longer to fail but hey it might get going.
1) if you have a remote load in the NL model it will not work, at leat in my experience - and yes the bug was filed many many releases ago - never know might be fixed. You would need to make up a component and just make it really stiff - and then see if you get past the fist step.
2) You need start managing the time step and the applied load vrs the predicted displacement at the first increment. If the item that is moving and will be restrained by only a contact, add a part and and bond the part to the moving bit, give it a material stiffness that is trivial in the big scheme of things but sufficient to give the unrestrained DOF some stiffness that you can predict at the first load step/increment. Make sure the displacement lies within some small fraction of the element thickness - like 5% then the contact can be detected and maybe it can get going.
After that it becomes a consulting project for me to figure it out.........good luck.
Oh and the global contact doesn't really matter much. The face specific contact will over ride it - the goabal is a default for coincident surfaces. If they are not coincident then they get nothing (no interaction - free). And sometimes, at least in my experience, for higher order geometry the default doesn't catch it. Also, if you set the deafult to contact it only support node to node contact - applicable only for normal force dominated problems (very little sliding) - if this is your situation then you want the faces coincident, whether it is a deault specification of a face specific one. Also, the component contact might not work so don't use it - bug filed for that as well.
Yeah you would not have to do this sort of thing with ABAQUS - pretty good contact, second only to MARC/MD NASTRAN in my humble opinion. Both those codes can get going without having to manage the initial conditions with a lot of effort. I have seen guys do just wild low stiffness contact with the MSC stuff. . Also, brick elements are a lot more robust for this sort of thing but you can get tet's to work - just depends on the situation.
To clarify, yes, it was at step #1.
Thanks a lot for your comments. I can see they are very valuable. I have made small progress by simulating only two components in contact but it takes long long time - I am talking about 10 or 20 hours with a simple model! I began to question the ability of SW on nonlinear stuff. Didn't have much help from our technical support either.
I don't have hands on experience on MSC even though I am pretty familar with the company/products. Don't know why they are a lot less popular than Abaqus or Ansys in US. I really love the seamless interface between CAD and simulation of SW over any other FE softwares, but their Nonlinear ...
Thanks a lot,