×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

FEA result - Local stress
3

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 winky smile
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

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.

RE: FEA result - Local stress

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.

RE: FEA result - Local stress

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.

RE: FEA result - Local stress

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  

RE: FEA result - Local stress

(OP)
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

RE: FEA result - Local stress

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) ?

RE: FEA result - Local stress

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.  

RE: FEA result - Local stress

(OP)
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

RE: FEA result - Local stress

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
www.espcomposites.com

RE: FEA result - Local stress

(OP)
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
 

RE: FEA result - Local stress

"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.

RE: FEA result - Local stress

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.

RE: FEA result - Local stress

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).

RE: FEA result - Local stress

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  

RE: FEA result - Local stress

(OP)
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 smile  

RE: FEA result - Local stress

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.

RE: FEA result - Local stress

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  

RE: FEA result - Local stress

(OP)
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

RE: FEA result - Local stress

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  

RE: FEA result - Local stress

isn't the permissible von mises stress = yield stress ??  why complicate it ???

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

(OP)
Hi there,
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

i think membrane stress is particularly relevent to pressure vessel design, and maybe not so much in your case.

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

The membrane stress is just the average stress across the section and is limited (usually) to 2/3 yield to prevent failure over the section through yielding (ie. a 50% safety factor). The type of element used will have no bearing on the calculation of the average stress across a section [presuming you have more than one element).

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

(OP)
Hi guys,
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

(OP)
I just need to add, in my handcalc's I calculated the bending stress and shear stress at the root of key boss shown in picture. and the max. stress in FEA is in conact edge of two components. and von mises stress at that point has been calculated.
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

Mohsen, a couple of comments:
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

how sharp are the pocket rads ? (in your model, and in the real part)

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 !?

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources