Convergence analysis of finite element analysis? 1

[bongirs]

Hello,

1. I have always done convergence analysis by checking the maximum stress for a scenario and seeing if it converges towards a value upon mesh refinement. However, my professor recommended a better method. He told me to choose a geometric point (x,y,x) and always have a node at this point upon mesh refinement. This point should be approximately in the area experiencing the maximum displacement. Now we check the convergence by measuring the values for this specific point instead of the max values. Is this method better than the max method? I think so, but just want to check the consensus over here.

2. Also, how does it matter if my parameter for checking convergence is displacement/strain/stress/strain energy?
I think displacement converges first and then strain and then stress and then strain energy.
But since numerical errors are introduced upon each conversion displacement -> strain -> stress -> strain energy, I think displacement is better suited for convergence analysis.

 

[ESPcomposites]

A convergence analysis will be specific to the variable you evaluating. In other words, performing a convergence analysis for displacement does not mean stresses are converged...and vice versa. Global and local effects must also be considered.

Consider a simple uniaxially loaded plate with a hole. At the location of maximum displacement, the mesh will show displacement convergence even if the Kt area is not highly refined. Therefore, approach (1) may fail if you are interested in stresses at the Kt.

Generically speaking, the maximum displacement is related to the overall mesh. Stresses are related to the mesh in the local region of interest (but the overall mesh must still be converged for the stresses to be valid).

Brian

http://www.espcomposites.com

 

[IceBreakerSours]

I agree with Brian.

And I would add the following: If you work with structured mesh topologies, then you must leverage the option of picking variables from the exact same geometric location for a true/fair assessment of how the variable is converging as the mesh is refined, if it is. With unstructured meshes, this can easily become impractical.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[bongirs]

Brian, I see what you are saying but I don't understand what better approach you would suggest?
Your argument about the Kt is correct, but as I said previously, the geometric point for displacement convergence is taken in an area experiencing almost the max stress.
So that way even for the Kt types of problems, it should work just as good.

IceBreakerSours, I understand that we should do convergence analysis for each parameter/variable we are analyzing. I find this interesting approach but still not convinced.
Let's say I am getting good convergence for displacement for a given mesh, then I should only take displacement from that analysis and no stress/strain?
Now what if the stress never converges upon further mesh refinement (but displacement already has)?

I also take it that you agree, we should consider a geometric point for convergence analysis instead of max values.

 

[ESPcomposites]

Just do a convergence analysis on the specific parameter you are interested in. Don't try to force it by saying that a stress based or displacement based approach is better.

To answer your question, doing a displacement convergence analysis at the point of max stress (Kt area) is not going to be the best approach. This is because the displacement is largely governed by the overall mesh and to a lesser degree by the local mesh. Conversely, the stress is more influenced by the local mesh and less so by the global mesh. Using the displacement to evaluate stresses would be like trying to accurately measure something small with a ruler instead of a caliper. Sure, both are used to measure the same thing, but one does a better job.

Also, if you use a displacement based approach, it will be ambiguous as to when convergence for the stress has been achieved. Exactly what displacement gradient between the different models indicates convergence? How could you convince yourself or someone else that convergence for the stress had indeed occurred? Conversely, a direct evaluation of the stress is relatively straightforward.

Brian

http://www.espcomposites.com

 

[bongirs]

Now I understand....
So you can choose stress as a parameter if you are checking local convergence and displacement if you are concerned about the whole body.
I can also deduct that in a local region if the stress converges then displacement also has to (in that local region only) ?
This is because in FEM the steps in calculations are displacement -> strain -> stress.
Please correct me if I am wrong.

 

[TGS4]

Not only that, but you need to consider WHERE the displacements and strain/stress is calculated. Displacement is at the nodes, while strain/stress is at the Gauss points.

 

[IceBreakerSours]

And you have to be careful with derived measures such as strain and stress because of extrapolation [from quadrature (Gauss or otherwise) points to nodes] and nodal averaging. Also, even though they show you several significant digits of precision for each of the derived measures, I have never found if the extrapolation and averaging are single or double precision operations - which may matter if, say, you are running highly nonlinear jobs with very accurate input parameters or if you were comparing your results against analytical solutions to a very high degree of accuracy.

If this isn't muddy enough already, here's another one for you: All jobs nowadays are multi-thread/node jobs, which - as it turns out - has its own challenges in that even the simplest of mathematical operations can be tricky. For instance, the sequence in which addition occurs can matter i.e., 1+2 need not necessarily be absolutely equal to 2+1 to the last significant digit.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[corus]

My guess is that the professor has in mind that stresses may simply continue to increase with a refined mesh at a point of singularity, say at a sharp corner or a point load, so continually refining the mesh would be pointless and checking for convergence of displacement would be a better option under those circumstances.

 

[ESPcomposites]

Corus, that is possible. But for something like a crack analysis, the stress slightly away from the singularity can STILL be used to determine a SIF (and it will converge). You would only have a problem at the actual singularity, but that is more of a fundamental understanding of FEM than a question about convergence conditions. If that really was the case, I would hope the professor would have explained that instead of talking about convergence criteria. Of course, something could get lost in translation.

Brian

http://www.espcomposites.com

 

[bongirs]

IceBreakerSours, do you really go into that level of precision in your analyses (1+2 not equal 2+1)? I always believe that FEA is good tool for giving you insight and not really anywhere close to reality. The Gauss point extrapolation is also why I never use stress/strain for convergence analysis.

Corus and Brian, the simulation that I am doing is a drop test of a fuel tank. There aren't much stress concentrations (or cracks for that matter) in my simulation. The thing is that we cannot go beyond a certain mesh refinement due to computational limitation. But we are still interested in understanding how much error could be introduced due to the incovergent mesh.

 

[IceBreakerSours]

I have seen first hand what horror such issues can bring; I lost a week of sleep in one such instance. The more nonlinear the problem, the more afraid and suspicious of solutions I become.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[corus]

The fact that the professor suggests using a point local to, but not at the maximum suggests that he/she has in mind the problem of singularity. If you're simulating a drop test then it's likely that the contact will be at a point and as such give you high stresses at that point that could not be resolved using mesh refinement. Hence they are suggesting a point close to this maximum position to check for convergence to give you greater confidence in the results.
As someone who has compared FE results to actual measurements you should find that FE results don't just give you an insight into the behaviour but can be very close to reality. In practice mesh refinement is the least of your problems for getting good results in comparison to real life.