Peak stress in solid FE models 5

[Struct71]

Hi all,

Does anyone have any guidelines or philosophies with respect to high peak stresses?

There are several guidelines to for design stress and maximum allowable stress for classic "manual" calculation methods, but I can't find anything for FEM/FEA maximum. How to deal with peak stresses?

Both as an engineer and as a checker I regularly find statements as

* "The high peak stresses should be ignored"
* "The maximum stress is local therefore allowable"
* "The hot-spots are negligible"
* "Due to the local nature of the high stress etc..."
* "Next to the red region there is a green region" (!!!)

As an engineer, this is not very satisfactory. Anybody else finds these situations? Is there a recognised guideline to handle peak stresses? How to evaluate them?

Hoping for a healthy discussion!

Regards,

 

[chaboche]

The plot in that last post didn't work, so here it is again:

 

[TGS4]

I just want to correct something that chaboche wrote in his previous post. He wrote that you can perform the fatigue analysis using the results of the non-linear analysis. If chaboche is referring the using the strains from said analysis, and comparing them to the ASME fatigue charts, then that would be WRONG!!!

In TF-EPFEA and SG-DA, we have been slowly working our way through how to do fatigue with non-linear analysis, and what I can tell you is that that is NOT the way to do things. The fatigue charts are based on elastically calculated stresses (hence the use of a K_e factor to adjust for plasticity), and comparing them with a non-linear analysis would simply not correlate.

 

[corus]

What is surprising in the last picture is that the results from the sub model don't appear to relate to the global model, in particular of the location of the maximum stress. I'd expect the results at the limits of the sub model to be the same (or close to) the results of the global model. I'd check that the displacements from the global model have been correctly transformed to the sub model.

You ask when a stress concentration becomes a mode of failure. I presume you mean by regard to some yield criteria and not by fatigue damage which the peak stresses at a concentration are assessed against. By defining the stress as that occuring at a concentration (or a feature) then you have already classified the stress and hence its limits. In terms of stresses away from the maximum stress at the concentration then you can look at the stress distribution up to and including the peak stress and attempt to fit a straight line through the stresses that will remove the non-linear contribution to the curve from the concentration. It is largely based upon your own judgement and so it would be better to err on the conservative side in your assessment. The resulting stress would be classed as secondary at the structural discontinuity. In the shell model this stress concentration of the fillet will be excluded and hence it would be better to assess the stresses as either secondary or primary based on their location. If in doubt then be conservative in your assessment and choose the lower limit.

corus

 

[chaboche]

I am interested to learn about the work TSG4 has done on non-linear fatigue.

Traditionally, the stress range during a cycle of a thermal transient can be calculated and compared against S-N data to give an allowable number of cycles. If pasticity effects are included in the FE model, why cannot the strain range be compared against the S-N data instead? This would remove the need for a conservative plasticity correction factor.


In response to corus, thanks for your comments. The reason for the difference in location of maximum stress between the global (shells) and submodel (solids) is due to the cut boundary interpolation. The maximum stress has shifted to the submodel boundary, where several of the shells are joined together. This has created a highly localised concentration. I have checked and the overall displacements between the models are in agreeement. Another contributing factor is that the shells weren't defined exactly through the centre of the solids i.e. some shells are located at the top/bottom of the solids. This was unfortunately decided before it was evident that a submodel would be required.

Regarding this location, you are correct that I wish to determine the strength of the section against a yield criterion, as opposed to the fatigue damage. I can see why the stress would be defined as a secondary stress according to a pressure vessel design code. Most structural steelwork codes however don't seem to classify stresses in the same way though. AISC or DNV, for instance just give limits on the calculated stresses without classifying them as primary or secondary (or maybe I'm looking in the wrong sections?). Is it therefore still valid to draw a line through the results to remove the peak?

A good way to show the stresses through the section is to plot those which are acceptable and those which are not. This is shown in the figure at the link below. It is then to be judged as to whether the concentration extends significantly enough to cause yielding of the entire section.

 

[corus]

The problem with structural codes, as I see it, is that they're based upon hand calculations of simple direct and bending stresses and don't consider the extent to which finite element methods can predict stresses. In fact I don't think they consider thermal stresses from what I remember. The pressure vessel codes do give more thorough ways of assessing stresses which the structural codes I've seen don't seem to possess.

Another aspect of peak stresses in transient thermal analyses to consider is the non-linear stress distribution through the thickness, which your 3D solid model will pick up. Your stress distribution might therefore be composed of this thermal stress component as well as the stress concentration from a geometric feature. You may need to calculate the equivalent linear bending stresses through the thickness of each section, and thus remove that peak component to leave only the secondary stress (range) and peak stress from the geometric feature. Effectively you'd have to extrapolate your results in two directions to remove any peak stress components.

In your case it's clear that the stresses at the fillet are due to the stress concentration of the geometry (plus perhaps a thermal peak stress). Stresses at 1.0t from the weld toe should be considered as nominal stresses and assessed accordingly.


corus

 

[gurmeet2003]

I would like to make one more comment on calculation of limit loads. This may be obvious to some. One knows the target factor of safety. In non-linear zone the factor of safety should be based on load and not stress. For example let us say that the factor of safety is 3. One could run another analysis with 3 times the load and look at the results. If the part has not yielded through the section, one may consider it safe. On the other hand if the run does not converge, it may indicate the part does not have the adequate factor of safety.

Gurmeet

 

[cbrn]

Hi,
yes, and in addition to what Gurmeet says, I'd add (just because I've seen it asked sometimes in Eng-tips threads...): when you perform a plastic analysis against direct collapse, you can not consider stresses in the plasticized zone: of course, they will be clipped to the yield value of the material (slightly more due to numerical reasons). You will have to:
- either compare the strains to related limits
- either perform a "limit-load" verification as suggested.

The important thing is that, in most cases, the direct collapse verification is subjected to strain limits by codes like EN-13445, not to limit-load safety factors (though these can be far more "understandable").

Regards