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

 

[rb1957]

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?

 

[Mohsen1979]

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

 

[rb1957]

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 ??

 

[corus]

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

 

[Mohsen1979]

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

 

[Mohsen1979]

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

 

[flash3780]

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.

 

[rb1957]

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 !?