Stress Singularity 3

[clsang]

Hi, all. I'm working on a linear elastic analysis.

The object I analyze is basically a steel plate with
some stiffeners. I model it with shell type elements.
I find out that the stress at sharp corners of
critical joint reports incredibly high. And the stress
value tends to increase endlessly against mesh size.
The smaller the mesh I model in this area, the higher
the stress I get. In that case, I can never achieve a
stress level below yield point of steel and I afraid
the final structure would be over designed indeed.

Is this something to do with gStress Singularityh.
If so, can anyone kindly explain what is gStress
Singularityh and how can we interpret our results in
light of this problem.

Appreciate you guys help.

Cheers

 

[zuardy]

Did you modell the stiffeners with shell elements also? How did you connect the stiffners to the plate?
Have you constrained the rotational shells DOF to their normal? Normally shell elements do not have this kind of stiffness, so if it is not constrained properly, it would lead to singularity.
As consideration : sometimes locally high stress region is acceptable.

regards

 

[prex]

Your problem occurs very often in FEA.
The point to be understood is that not all the stresses count and need be limited in the same way. As an example, when you calculate a common frame or truss structure with beam elements, you totally dismiss the local stress distributions at the joints, that might be done for example with stiffened flanges and bolts: those local stresses are normally even not determined by the designer, but of course they are there!
I'm sure that you are facing a problem of this kind. The bad news is that to determine which stresses are relevant one needs to know in detail how the structure works: so I'm afraid I can't give any more advice at this point. prex
motori@xcalcsREMOVE.com

http://www.xcalcs.com

Online tools for structural design

 

[clsang]

Thanks for the reply.

Zuardy. Yes, I model the stiffeners with shell element also. I constrained all the six DOF of shell elements at the fastening area. Is that enough or as you said, I have to constrained the rotational shells DOF to their normal. But I don't found high stress at this area. The high stress gradient happens at the joints of horizontal and vertical stiffeners.

Regards
Clsang

 

[DarrellW]

clsang,
I'm not an FEA mathematician so I have to go along with what the the Post Hole Diggers in the profession say about it and hope I understand enough to get along. To make a long story short, I tend to think of 90 degree FEA joints with no fillet as places where the continuity equations have to solve x/cos90 in order to make X strain out of Y strain. Of course the software has to make an approximation at the "divide by zero" point which could be a very large number. Thankfully, St. Vennant's principle comes to our rescue in the real world and at some distance away and everything is well behaved again.

I have had good luck in ANSYS in many of my evaluations by believing stress values that would be the equivalent of 2/3 to 1 fillet length away from the fillet root, possibly less. This is dependent, of course, on mesh size and is sort of where the science becomes art. If you see a general stress state that extends out some distance from a fillet, then you darn well know the fillet sees at least that much stress. Remember that in very sharp corners, a stress concentration factor of 3 or 4 may be applicable. If you indeed do have a very near 90 degree joint and need to know the precise stresses in close proximity, then you should probably go to a local analysis, model the exact geometry, and then solid model it.

Hope this helps.
DarrellW

 

[clsang]

DarellW,

Thanks for your valuable advice.

Best regards
clsang

 

[FeaGuru]

Blah blah, the stress is there. If your geometry is truly sharp, then expect high stress. But ya know what, there is thing called plasticity. This may or may not be a big deal, but what should be looked at is the type of material (mostly its ductility) and what type of fatigue loading you expect.

 

[KSWpe]

FeaGuru is right. If you have an inside corner, you're going to have infinite stress at that point - and the more you refine the grid the more you will approach infinity. That's where you have to make engineering judgements as to whether the stress raiser is a problem for brittle parts, fatigue, etc.

 

[idly123]

Well that was a good querry. I have a set of points to share
from theoretical aspect.

1) When u talk of a renetrant corner(90 deg bend or a stress singular zone).u r results are not likely to converge .this is very clear.
two issues face us
a) it is required to get the accurate stresses at the point
b) what is the influence of further refinement on stress value
2) By progressive refinement of a FE Mesh we tend toward a consatnt strain state. Irrespective of elemnt order this takes place. So what stress we us eis a question

The answer is:

For lower refinement , that is for initial meshes go for stresses obtained from higher order derivatives of displacements.

For higher refinements, fine mesh, go for lower order derivatives of displacements to obtain stresses.
(refer to a paper by BArlow IJNME 1995)

To get a more precise and accurate value of stress u need to perform an error analysis (Zeinkewicz and Zhu paper would help)

hope this helps u in some theoreticcal understanding rather from using a package. I havent worked on a package so i dont know the difficultie din that
regds
raj