Ansy Convergence Criterion 5

[Nildev]

Hi, Please let me know if somebody has info for the below
In one of my problem I had nlgeom,contacts and nonlinear mps. Problem was difficult to converge with default CNVTOL. I thought to relax. With only moment convergence(1e-4) very small I could get convergence. But Ansys recommndes F and M together(Together I could not get the convergence). I would like to know what are implications of each one. How much difference in results(approximately) percentage one should expect by using different CNVTOL. Please let me know if you have any document on this. I had done my search on Ansys.net. I could not get any document on this.

Thanks in Advance

 

[cloche]

VERY difficult to answear exactly, I fear!
If not checking for force convergence, you should verify the force unbalance of your model by looking at the reactions: if the react force summation is near (how much depends on your own analysis citeria...) the loading forces' summation, then you can accept the solution, otherwise not: remember that a FEM is a displacement-based solution, so the forces depend on the displacements guessed at each iteration, then forces are compared to expected force balance; if you don't want the program make this for you, you have to do it by yourself in some way or your model could have converged but be "on planet Mars" !!!
Based on my personal experience, one of the most difficult "things" to set are contact parameters: try leaving the default convergence criteria and work on your contacts: I'm pretty sure you will find out something in them that causes the non-convergence (Gauss-points slipping in/out of contact unexpectedly, normal or tangent slip tolerances too stiff, penetration tolerance too small, etc etc...). The number of tools you can use to check what happens to the contacts is very high, only this topic could fill a new thread !
Or, due to the fact that you have geo nl, possibly your model is getting unstable at a certain point: track your convergence history, then try to do several loadsteps by stopping the first right before the original source of non-convergence, or diminish the timestep.
Anyway, non-conv on force balance, when moment-conv is achieved, generally means a problem somewhere in the model with translation DOFs: it could be due to geo nl (large displacements / large deformations...), material nl (elasto-plastic material could have overcome its strength limit, leading to VERY high displacements - remember that any table-definition of whatever property must extend beyond the analysis range, as a table can only be interpolated and never extrapolated), contacts, or a combination of everything (!)...

Claudio

 

[Nildev]

Claudio,

Thanks for detailed explaination. Your explaination about Force balance is very much convincing me. Few of the things from above I have already tried. One thing which is not in control is material data limits.
As you pointed out: the forces are such that the stresses calculated exceeds table limits. But still I would like to see the max stress value, and area or zone which exceeds the ultimate? Is it possible-Like in linear material property analysis we will able to see the stresses which are above the yield or ultimate. Similar thing by using nonlinear material properties.

Thanks in Advance.

 

[cloche]

Ehm... too difficult for me ;-) I would do this "by hand", i.e. fictitiously extend material data table beyond strength limit using low E value; then, once the analysis has been run, whenever you see strains larger than the ultimate strain then your material would have broken in reality. A very sophisticated solution I've never tried, is to stop the solution at limit point, then use "birth" and "death" of some elements in order to simulate the birth of a crack, then give "restart" and analyze crack propagation... Provided that you have an idea of the initial crack shape! ;-)

Claudio

 

[Drej]

Nildev - see my previous thread on this subject thread569-123268. We have discussed this previously. You cannot give a definite answer regarding the implications of each criteria, as the results depend on the type of analysis, and the way in which it is loaded. This is why ANSYS changes convergence limits/types dependent on the type of analysis carried out.

> How much difference in results(approximately) percentage one should expect by using different CNVTOL.

Impossible to answer. If you have a large tolerance your residuals will be large. If these accumulate throughout a multi-step analysis, the error could be huge.

Claudio

> If not checking for force convergence, you should verify the force unbalance of your model by looking at the reactions: if the react force summation is near (how much depends on your own analysis citeria...) the loading forces' summation, then you can accept the solution, otherwise not: remember that a FEM is a displacement-based solution, so the forces depend on the displacements guessed at each iteration, then forces are compared to expected force balance; if you don't want the program make this for you, you have to do it by yourself in some way or your model could have converged but be "on planet Mars" !!!

Be careful here. Your reactions should ALWAYS balance, regardless of the type of convergence used. Force convergence does not guarantee that your reactions will balance. This is another issue altogether. You cannot accept the solution being accurate based on the summation of reactions equalling the applied loads. Absolutely not in the context you are describing. Checking the reactions is a basic check of your model and should always be carried out. If your convergence tolerance is based on displacement, and your residual is 50% of the applied displacement, your reactions may sum correctly, but your displacements may be enormous (and most definitely incorrect). As I've said previously, you must base your convergence criteria on something other than is applied: e.g. you apply a displacement in your model, you should converge using forces (and moments if necessary) etc.

Nildev

> As you pointed out: the forces are such that the stresses calculated exceeds table limits. But still I would like to see the max stress value, and area or zone which exceeds the ultimate? Is it possible-Like in linear material property analysis we will able to see the stresses which are above the yield or ultimate. Similar thing by using nonlinear material properties

This I don't understand. If you want to see the max stress of an area you need to consider both von Mises or a component of Principal stress. You don't need to worry whether your material properties aren't non-linear, as the stress shown will be based on the data given. If you're doing a linear analysis, then you should consider looking at von Mises or Principals (depends on the type of analysis). If you want to model plasticity, then you will need to produce a table (TB) of non-linear data.

 

[Nildev]

Hi Claudio and Drej,
Thanks for keeping discussion live and useful. I am sure there is no perfect answer for this, but discussion will evolve
1) Points to check if we are using our own tolerances
2) Which Criterion to be considered?
3) Convergence issues with Nlgeom and Nlmaterial.

Cluadio,
Your suggestion about birth and death is appropriate. But it is again dependent on so many things and it is more complex(Atleast for me). Is there a way/methodology we can extrapolate the curve and make ANSYS understand dummy stress strain behaviour above the ultimate stress.

Drej,
About our last point, what we are looking is
If we use nonlinear material data: max stress in your model can be the highest stress value which you had entereded in the stress strain curve. Let us say your ultimate is 100ksi, then model will have max stress of 100ksi. But if you do a linear analysis you can even see 200ksi or 300ksi..There is no limit on max stress. With linear analysis you can see how much region goes above yiled or ultimate. Same way we were trying to know any equivalnet if we use nonlinear mps.

 

[cloche]

Hi all,

I also think that this discussion is getting very interesting, but I also fear that we're losing contact with the practical problem...
1) Drej, you're right; my first answer was inaccurate. But a complete answer would need to involve analysis of FEM methodology (matrix inversion, trial-and-error algorythms, etc... The basic concept is that in the complex scenario described, full of non-linearities of any kind, the relation between displacement pattern and force-equilibrated distribution pattern is not a bijection any more, and is "search-path"-dependent. In linear static instead we are in a "happy island" where given an equilibrated force distribution there is only one compatible displacements pattern, and/or given a coherent compatible displacement pattern there is only one force distribution that can equilibrate it. Drej correctly points out that in non-linear, this is NOT necessarily true...

2) I think we always have to compare with the real physical world: real world will tell if displacements/forces we find are "possible" (otherwise, how could I decide if I can accept the solution? look at the residuals? sure, but if I had to loosen the criteria, I myself forced these residuals to grow up! So they are not an ABSOLUTE indicator, I fear. I can find cases where 1% residual error on force/displacement is too high, and also cases where I can accept more than 10% residual error...). Can we find a guideline with which to decide when to consider a solution "acceptable" and when not? Similar real cases? Ratio btw values (which ones?). For the moment I always knew similar cases to compare my new analyses with, so I was a bit lucky if you want...

3) I also believe that we must not ask "too much" to the program: we don't want to become automates ourselves. If we know where to set the limits, there is no necessity to get the program have a criterium for us: if, given that the solution itself can be accepted as "conveniently accurate", I see that the only displacement pattern which is compatible with my force field involves 120% strain in some point of my model, and I know that my material can only endure 95% strain, then I am done: the material has failed, there is no chance but to change something in my design. To be precise: the material has failed in THAT point; it doesn't necessarily mean that the component has failed as a whole: it surely gets damaged, but then the defect propagation depends, once again, on the force field.

Claudio