FEA result - Local stress
FEA result - Local stress
(OP)
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
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





RE: FEA result - Local stress
Ed.R.
RE: FEA result - Local stress
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.
RE: FEA result - Local stress
RE: FEA result - Local stress
Tata
RE: FEA result - Local stress
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
RE: FEA result - Local stress
RE: FEA result - Local stress
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.
RE: FEA result - Local stress
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
RE: FEA result - Local stress
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
www.espcomposites.com
RE: FEA result - Local stress
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
RE: FEA result - Local stress
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.
RE: FEA result - Local stress
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.
RE: FEA result - Local stress
RE: FEA result - Local stress
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
RE: FEA result - Local stress
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
RE: FEA result - Local stress
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.
RE: FEA result - Local stress
Tata
RE: FEA result - Local stress
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
RE: FEA result - Local stress
Tata
RE: FEA result - Local stress
take your von mises plot, maximum less than yield = GTG, no?
btw, somewhere in the calc you have taken care of the appropriate safety factors, yes?
RE: FEA result - Local stress
I found a nice procedure for stress analysis in a standard AS1210. This standard is a pressure vessle design code and I just wondered if it is applicable for general purpose stress analysis?
Based on that, the stress is categorized in 5 groups as follows:
1- General primary membrane stress
2- Local primary membrane stress
3- General & Local primary membrane plus primary bending stress
4- Primary plus secondary stress
5- Peak stress
And each category has specific limit for check. At this standard the limits for pressure vessel design case has been nominated.I need to add, all stresses are stress intensity (twice Max shear stress) and Tresca theory.
I think this procedure can be used for any general stress analysis if, firstly, I can categorize the stress to those caregories and secondly, the right limit for each category is available.
How do you think? Please add your comments here
thanks in advanced,
Mohsen
RE: FEA result - Local stress
in any case, how do you get membrane stress from TET output ?
why not just use von mises output from the TET elements ??
RE: FEA result - Local stress
I'd use the pressure vessel code method for FEA results, but at the same time I'd also satisfy the structural design code limits for the more general direct (ie. membrane) and bending stress limits, where the direct + bending stress would be the surface stress away from discontinuities.
Tata but not yet tara
RE: FEA result - Local stress
Thanks for your comments, But still I'm confused. These day I've seen different documents and procedure, but i could not the answer of my question.
So I just decided to ask my question as simple as possible and show that as an example.
please have a look at the picture attached to this post and give me your comments,
Cheers
RE: FEA result - Local stress
As a question, is a static analysis is correct for this problem. I mean the high stress is at the contact edge.
cheers
RE: FEA result - Local stress
1. The picture that you posted on Dec 10th is showing a singularity. If you refine your mesh, the stress will continue to rise in an elastic model. The best way to determine the stress in that region would be to create a sub-model with a minimum of 5-8 elements around the radius. The second best way would be to find the nodal loading, compute the normal and shear stresses, and apply stress concentrations from handbooks (i.e. Peterson's). Reporting the results as they're shown is incorrect, as the value is dependent on the mesh density. As was mentioned previously, concentrated stresses are generally not of great concern for one-time static loading in ductile metals, but may initiate cracks for a fatigue failure.
2. As for the second figure you posted. You asked about the fixed boundary condition that you have applied. Yes, this will produce higher stresses than the part sees. The best way to determine the stresses at the interface would be to model the mating part with a nonlinear contact. It looks as though you've highlighted several other stresses in sharp edges. To determine the concentrated stresses, you'll need to model the fillets (again, probably in a sub-model), or you may compute the concentrated stresses from the nodal forces and a handbook (as described above).
3. I'd wager that a static analysis is fine for this model. If you want to run a harmonic analysis, you'll need to do follow-on work.
RE: FEA result - Local stress
i suspect you might have suspressed these to help the modelling. if the modelled corners are unrealistic, then the results are conservative.
in any case, for my money, if the peak nodal averaged von mises stress is less than yield i think you're GTG. if the element averaged vM is less than yoeld, i'd probably buy that too.
as falsh noted above, your BCs will have an impact on your results, for better or for worse !?