Why no convergence?

[trainguy]

Once again, I turn to the experts:

In my never-ending (no pun intended - see below)analysis of a passenger railcar, the same one I've been crying about in my last 10 posts, there is a strange occurance -

The NL elasto-plastic analysis is set up in 20 increments; 10 to get to full load, and 10 more to get back to the unloaded condition. The analysis runs fine, (i.e. converges within the max. no. of iterations, etc) up to full load, and then even down to the 18th increment, at approx. 10 % of full load. At that point, the analysis never completes, it just keeps iterating, with apparent divergence, as the max. displacement reported keeps on increasing.

Does this imply structural failure? The fully loaded step gives apparently good results with regard to stress distribution, and reported plastic strains. The FE code is NE/Nastran.

It would be really nice to be able to report residual plastic strains, if they're calculated correctly.

Thanks in advance,
GA

 

[EdR]

trainguy:

This one has me confused since unloading is generally an elastic phenomona and there is no good reason for displacements to continue to increase....Unless you find some modeling error or material property/loading error I would not trust the results and do not see how they could imply structural failure...

If you are in fact applying some additional loads in an attempt to reverse plastic deformations them maybe but just removing a previously applied load should not cause this type of behaviour...At least for any condition I can think of....

Ed.R.

 

[EdR]

trainguy:

It occurs to me that you should check the unloading steps that you initially have for large displacement changes as well as plastic strain increments....If you see inelastic behaviour on initial unloading steps you have some sort of problem with the material model definition or some other unloading related problem...

Ed.R.

 

[brad]

One misteke that I've seen people make:
Many people will prescribe in the first step a load of, say, +100, then in the second step a load of -100. Most (maybe all) nonlinear FEA codes utilize by default the ABSOLUTE VALUE of the load; not a relative value.

The proper way to model loading and unloading would be a load of +100 followed by a "load" of "0" in the second step. If your second step has a load of -100 instead, this is in fact a reversal of load, rather than an unloading. This could certainly lead to the behavior you are describing.

Just a thought.
Brad

 

[corus]

I could imagine this as one section being subject to the dominant elastic behaviour of the surrounding structure. As the elastic structure deforms, one section deforms plastically with it. As the elastic structure is unloaded, the plastic section buckles under the surrounding strain determined conditions rather than load determined conditions.

 

[brad]

corus,
While your suggestion is physically possible, I think I
have only ever seen it once.

I have seen the above-described behavior at least a dozen times (from helping others). Every time I have seen was due to either a misunderstanding of load application (differential load vs. absolute), or else problems with convergence criteria as the load (the denominator in load residual calculations) gets very small. This is what I believe Rakesh is alluding to.

The latter does not generally manifest itself as divergent displacement, but rather as simple convergence failure on the force equilibrium (but with converged displacements).

 

[corus]

To add to my previous note I would suggest that Trainguy looks at his results to see where the divergence of displacements is occurring. If the results are saved per iteration then the displaced shape could be viewed to give a clue as to the cause of the non-convergence as this may only be occurring at a single node, as is often the case. That is, presuming that the loads have been apllied correctly as Brad suggests.

 

[trainguy]

Thanks for responding, everyone.

The loads are applied fully in the 1st subcase (10 increments) and are 0 in the next subcase, as per NE/Nastran's support suggestion. They felt that using small non-zero loads was unnecessary.

In my definition of material properties, I used one fictitious material with E=2000 MPa (instead of 200 000), while setting G=77000 MPa, in order to work in shear only. My FE analyst at the time was not comfortable with shear only elements. Could this be to blame?

 

[EdR]

trainguy:

This material property is definitely giving you bad results in the elastic range which feeds back into the solution through the stresses, etc....For E=2000 Mpa and G=77000 Mpa poissons ratio is -.9870...(G=E/(2(1+nu)) elastically....This will give squirrelly results locally and could screw up the overall results as well.....

Ed.R.

 

[brad]

Train Guy--Bad IDEA!
The phoney E will possibly do three things (one of which EdR suggests above). The other two:
1) You will likely have matrix illconditioning problems due to the large relative difference in the stiffnesses.
2) I'm not sure what to make of the craziness that will result in the plastic calculations of this material. This is very likely the source of your problem. The plasticity algorithm will track, but I can't off the top of my head speculate as to what may happen. My money is on this as the source of your problem.
You need to do a "true" shear element, if you can (although I don't know whether this is directly possible within NE/Nastran, as I am not familiar with that particular flavor of Nastran). You really should rethink this approach to shear elements.
Brad

 

[trainguy]

This approach, while shocking to true FEA professionals, actually gave decent results in linear static runs, or so the contour plots showed. Thin sheets did not carry significant load, and their stiffening channels and zees carried most of the load. Results related quite well with manual calcs!

For your info, this (Low E) material was not assigned any plasticity. It was a strictly linear material. We used this approach after the first linear runs (assuming a fully stable cross-section) showed panels carrying stresses which exceeded their buckling stress. I guess we really should have explored the shear only elements more closely...

 

[brad]

I understood that this was within the area that was yielding. This is not so bad if this was not assigned plastic material properties. I would still recommend using a shear-element, if it is available in the code.

Methods such as what you have done are common in linear analysis (another example is modeling something as "stiff" by increasing E by 10^6). These approaches, while harmless in linear analysis, often cause problems in nonlinear analysis due to matrix ill-conditioning issues (mentioned above). So even though it gives reasonable results, it may still be behind convergence issues (but maybe not).

Brad

 

[MarcoE]

The most likely culprit of divergence in FEMing is inadequate meshing. This can be from not choosing a small enough element size for small geometries or improper arrangements of nodes around stress concentration points.