FEA result - Local stress 3

[Mohsen1979]

Hi there,
I got a question and I really appreciate if someone could give me some idea. Thanks in advanced ;-)
My questio is about evaluate of FEA result of structures. Infact, there are some localized high stress area in the FEA result, for instance, at the filet welded area of two perpendicular member the stress is 300MPa and other parts of structure the stress is 60MPa. In otherwords, just 0.1% of elements of the structure are more than 60MPa.
I'm a bit confused how I can conclud the FEA analysis. I like to know if this situation is acceptable or not.

And if you know any references that can help me to understand this matter, please introduce me.

Cheers

 

[EdR]

Without more information there is no way anyone can answer your question.....It could be real if it is in an area of stress concentration and is modeled properly but more likely it is some kind of mistake in your model or just a poorly modeled structure. There is no way for us to know......

Ed.R.

 

[rb1957]

agree with Ed ...
i have accepted local hot spots 'cause they are local and a limited amount of yielding will eliminate the problem; but without detailed info, we can't assess your problem.

 

[kan123]

There are also some geometries and loading conditions that can cause a singularity no matter how well you model the structure. This would cause a local high stress that will not converge with increasing mesh density. If the material is ductile and the predicted yield zone is very small, you can probably justify ignoring the predicted maximum when assessing the risk of permanent deformation or ultimate failure. However, if you are doing a fatigue analysis, you may need to use an approach to estimate the maximum stress or strain to use in your calculations. This might be done by ignoring the questionable region and extrapolating from the reliable results. Determining what is "reliable" might entail doing some sort of mesh density study.

 

[corus]

If it's local then it's called a 'hot spot' stress. Google that term for evaluation of these stresses. It's classed as a peak stress likely to cause fatigue damage.

Tata

 

[Mohsen1979]

Thanks all for answering.
I've attached a picture of that situation I explained.
In this case, at the corner of welded edges, the stress is about twice of the permissable stress (based on the standard). The material is 6061 - T6.
Could you please give me some idea about this matter.


Cheers

 

[rb1957]

IMHO it looks like an artifice of the model (and probably not something real) ... what if you bevelled the edge off the model (and maybe off the finished weld too) ?

 

[EdR]

Could be what RB describes.....I really can't tell from the picture but if my eyes are seeing correctly it appears that the area may be an area of stress concentration.....I would suggest you take the structural dimensions and a text (Roark maybe) and investigate what kind of stresses you get from considering the stress concentration factors, etc.

This should give you a better idea of whether its a problem with the model (which appears less likely to me after seeing a picture unless you have made hand modifications in this area of the model) or whether it is real.....

Ed.R.

 

[Mohsen1979]

RB1957, thanks for ur comment.
I couldn't understand what you mean about real model. That's the CAD model of the part has been design and the bevelled edge are the weld and meshed as solid.
Could u please explain more about the proper model for FEA.
Cheers

 

[ESPcomposites]

The FEM is doing what you told it to do, which is to capture the Kt of a sharp corner.

This problem can be addressed by one of two ways:

- If you actually do care about the Kt (i.e. brittle material, composite, or metal fatigue), then you should model with with the actual geometry (i.e. not likely a sharp corner) to get the desired Kt. You would then use the Kt result to determine failure.

- If you are looking at the static failure of a ductile material, the Kt effect will "go away" as the material yields and does not have any effect to failure (or very minor).

A link that may help.

http://machinedesign.com/print/74495

Brian

http://www.espcomposites.com

 

[Mohsen1979]

Ed.R, thanks for ur comments.
I like to know what will happen in real situation. At that area the stress is high, two peices of the part is welded.

I found that in real situation, there are some plastic deformation in a such area with high stress and after that the stress will be released. But I don't have any references for tis point. Do you have any idea in this matter.
Cheers

 

[rb1957]

"real" refers to the stresses in the real part; as opposed to stresses in the FEM part. i think the FE thinks that the sharp corner (as modelled) is attracting more load than i think it would in reality.

put another way, if this corner yielded, what would happen to the loadpaths of the part ? there is alot of lightly stressed material around this "hot spot" which would (IMHO) support the more highly stressed corner.

as i said, try bevelling the corner off the (model) part and see what happens.

 

[EdR]

I guess I'm no longer sure what you are asking....As both rb & esp have indicated, and indeed what you said in your last post, if the stress in the corner exceeds the yield stress then plastic deformation will occur and the loads will be redistributed. If you can accept this inelastic behavior in the part then fine, if not then you must do something to reduce the stress concentration such as rb suggested i.e. bevel the corner.......

Also note that the stress is not "released" when yielding occurs. What happens is that the stress takes on its maximum value (the yield stress) and additional areas have a stress increase until the load is redistributed.

Note that to get a better feel for how the redistribution occurs and how much deflection is associated with the yielding you would have to run a material nonlinear analysis.

Ed.R.

 

[kan123]

Since your peak stress is well above the yield point, a stress-based fatigue calculation probably might not show as much margin as you want. In that case, you would have to use a strain-based approach (such as one of the models proposed by Manson: A Modified Universal Slopes Equation for Estimation of Fatigue Characteristics of Metals, U. Muralidharan and S. S. Manson, Journal of Engineering Materials and Technology, January 1988, Vol. 110/55).

 

[corus]

The permissible stress isn't just the yield stress, or whatever, but depends upon its location and type. Design codes generally tell you how to classify stresses and based upon that classification give you the permissible stress. In this case it's obviously a localised peak stress where normal permissbile limits don't apply but a fatigue assessment does.
Personally I regard any stresses coming from tetrahedral elements as being suspect in regard to values of localised stresses unless you put a significant amount of elements in that location. If you don't have cyclic loading then forget it, otherwise use a local model of that area, or estimate the peak stress from the nominal stresses in that area coupled with a formula for that stress concentration from Roark, say.

Tata

 

[Mohsen1979]

Thanks all friends, your comments has been usefull.

As another question in this subject; I like to know how we can connect the result of FEA with the permissable stress nominated in the codes and standards. For example, in the standard I'm using, has been mentioned:
For combination of tension and bending load, the acceptable condition is : Sn/0.6SY + Sbx/0.66SY + Sby/0.66SY < 1
Sn : Normal Stress
Sbx: Bending stress in X direction
Sby : Bending stress in Y direction

I like ti know how I connect the stress plot of FEA to this criteria.

Please give me some idea in this matter.

Cheers

 

[rb1957]

since you're modelling with solid elements all you get is local stress, you don't get sress due to tension, etc.

i don't think it makes sense to drive tension and bending on the critical TET element based on the stresss fom the element, eg average stress = Sn.

i'd replace the allowable 0.66Sy with 0.6Sy so your conditon becomes s/(0.6Sy) < 1, or s < 0.6Sy.

 

[corus]

Those limits seem more applicable to structural codes for beams or sections where the stresses have been derived by hand. You could use some linearisation method to derive the mean and bending stress across a section of your model and apply those limits but it may be too complex for your particular model. In general it's better to assess the mean stress across a section, ie. the membrane stress and apply limits to that. The surface stress without the peak stress due to the concentration would be the membrane plus bending, which will have a separate limit (usually yield stress). You'll have to remove the peak component by linearising the distribution, somehow. Of course if the total stress (including the peak) is less than the limit then there's no problem.

Tata

 

[Mohsen1979]

Rb1957, Corus,
Thanks for your comments,
Let me ask my question in another way. I like to know how I should report the result of FEA in accordance with a specific codes.

Is that right that I define a permissable von misses stress based on the standard, for example:
Sn = 0.6 SY
t = 0.45 SY
then calculate von misses stress as :SQRT(Sn^2 + 3t^2)
for a simplified plane stress (surface stress)
And then compare the von misses stress plot of FEA with this calculated permissable von misses stress.

Cheers

 

[corus]

Taking your expression SQRT(Sn^2 + 3t^2) the limit for Von Mises works out at 0.98.Ys, ie. approximately equal to the yield stress. The limits you'd apply to your model would be Yield stress on the surface, and 0.65Ys for the mean stress through the section. At the peak stress positions it is clear that those limits don't apply as such as they include a stress concentration. If you look at your contour plots though you can see that the stress distribution is all over the place at those peak positions, and missing at other places where you'd expect to see a peak, Tet elements aren;t much use for these types of details alas, I'd ignore those peak values and put them down to a combination of mesh sensitivity and stress concentration.

Tata