Stress concentration on a curve 1

[Twoballcane]

Hello All,

Let’s assume that an angle iron’s sides are being squeezed towards each other and pivoting at the elbow. On the stress plot you can see the stresses on the outside and inside part of the elbow. Now, some time in the past I do remember reading an article about stress concentration in FEAs. That the nodes on the curve, because of the math, will calculate higher stress than what might be really happening, it also said that to get a good estimate of “true” stress to read the surrounding nodes near the curve. So in the end, the highest stress in the legend is not what you want to take as max, but the next level down from the top.

Can somebody tell me if I’m imaging this, because I can not find any info on this on the web?

Also, I use Pro Mechanica if that helps.

Thanks


Tobalcane
"If you avoid failure, you also avoid success."

 

[corus]

I've never heard of this before, and seems to be a lame excuse not to take the maximum stress shown in the results. Stress convergence is usually monotonic and from below the 'true' value. What you've probably read is that at a stress concentration, such as at a 90 degree juncture, then the stress at the corner will tend towards infinity and for fatigue assessment you'll take a nominal stress value some distance away from that corner.

corus

 

[rb1957]

i'm with corus, though alittle less "lame" ... the stress peak is on the surface and the peak is very sharp (the stress gradient is very high). thus in most cases there'll be plasticity occurring, very, very localised and not significant. so the maximum stress predicted by linear FEA is consersative, and the real stress peak is less ('cause the real world isn't linear). depending on the situation you could talk away a localised stress peak, you might use element centroidal stresses.

 

[EddyC]

My Roarks 7th edition seems to have the case that you described. They give a range of Kt depending upon the size of the angle being used.

 

[corus]

rb1957 has a point about plasticity. The real stress at the concentration would of course be the yield stress value, but there would also be a redistribution of load around the yield surface, which would alter the stresses in that region. In any case, taking a stress at the next element away is bad practice as then your results are dependent upon the mesh. Similarly I wouldn't take the stress at the element centroid, as although it's calculated more accurately there, it's only more accurate for that position.
If the stress is at a corner then high stresses at that location don't necessarily mean the structure fails even if the stresses are above yield. Localised stresses should be considered as causing damage through stress cycling, leading to fatigue damage.

corus

 

[ktop]

On the stress plot you can see the stresses on the outside and inside part of the elbow. ...stress concentration in FEAs. That the nodes on the curve, because of the math, will calculate higher stress than what might be really happening,

This depends on your model. From the sound of it you modeled the angle with 3D elements. If you had modeled with shell elements what you say would be true because the corner where the two legs come together is a singularity of sorts.

But if you did a solid model using 3D element (tets or bricks) then all other things being equal your model is showing the correct stresses. Of course if you are yielding you will have to account for that with a non-linear analysis.

You have to pay attention to the sense of the stress. Is it compressive or tensile? vonMises won't tell you that.

BTW, many times FEA is used to calculate stress concentrations. Just remember that FEA does not give engineering stress, it gives true stress.

KTOP

 

[rb1957]

i'd go further than ktop ... if you're using a 2D element model, you've no hope of actuately calculating the local stress at the junction of the two flanges of the angle. a 3D model at least allows you to accurately model the details.

 

[Twoballcane]

Thanks everybody for participating in this thread.

I guess I picked up a bad habit, but I’m not alone:

http://www.eng-tips.com/viewthread.cfm?qid=211759&page=14

I could of sworn that I read somewhere that the peak localized stress can be neglected due to the math. Where stress is calculated through out the nodes and once it starts to concentrate onto one or two nodes at the curve the stress goes up exponentially. So the nodes closes to the peak stress are acutely close to actual stress. In ProM we use Von Mises. When I do my Von Mises hand calcs, it always comes lower than what I have as max in ProM. However, in any case, I will take the max stress as actual stress and make sure the geometry and mesh are appropriate.


Tobalcane
"If you avoid failure, you also avoid success."

 

[rb1957]

"In ProM we use Von Mises." ... you don't Have to ... i'm sure you can output max/min principal.

"When I do my Von Mises hand calcs, it always comes lower than what I have as max in ProM." ... doesn't that sound like a problem ? mind you the von Mises output could be derived from an intermediate stress result, and it could be inconsistent with the principal stresses (or the nodal stresses) you're using to hand calc it.

 

[johnhors]

At stress concentrations in complex geometry either the maximum or minimum principal stress will be greater in magnitude than Von Mises. This is not a problem it is normal. Relying solely on Von Mises can be dangerous, it is a yield criteria and should be used as such. For strength it is much safer to use principal stresses.

 

[rb1957]

i read the post to say the hand calc'd von Mises is less than the machine calc'd vM ...

if the principals are all +ve then vM < s1 (the max. principal)

i agree about preferring max principal over vM as a failure criteria, partially 'cause vM is a yield (linear) criteria. that said i don't think it that "dangerous" ... it's probably conservative 'cause it doesn't account for plastic strain energy.

 

[Twoballcane]

Yes, I am using the distortion theory as my failure criteria for yield, however, I thought this was the best way to evaluate ductile material because you will take in consideration of all three max principal stresses?

Tobalcane
"If you avoid failure, you also avoid success."

 

[kellnerp]

You still didn't answer the question. Shell elements or solid elements?

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[rb1957]

"don't wait for the translation, answer the question !"

 

[Twoballcane]

oh Im sorry, solid elements....

Tobalcane
"If you avoid failure, you also avoid success."

 

[kellnerp]

OK, solid elements. How many through the thickness in the angle iron?


TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[Twoballcane]

Hi Kellnerp,

In the op, this was an assumption for an example to speak too. I typically do solid elements when I do ProM. My question was about peak stress and what to do with them. But, I want to thank you for your time participating on this thread. What is your opinion on peak stress?



Tobalcane
"If you avoid failure, you also avoid success."

 

[kellnerp]

You have to look at the stress gradient. That is why I asked how many elements through the thickness. The other question is whether you modeled the actual profile of an angle or just have a sharp corner on the inside.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."