Stress in point of discontinuity

[AndyLake]

The stress in the point of discontinuity (for example, the corner of the structure) depends on the size of the shell element (smaller element -> higher stress). Is it impossible to solve exactly the stress in the point of discontinuity (by using the shell elements)?

 

[johnhors]

Yes ! Type of element is irrelevant. A sharp corner is a singularity with no exact solution, and in reality does not exist. Every edge or corner has a fillet radius, which can be meshed fairly accurately to get a good estimate of stress. Obviously the tighter the radius the higher the stress.

 

[rb1957]

would a non-linear analysis help ? i mean there'd be local yielding at the notch ...

btw, to beginner77; FEA will only give approximate stresses. usually the approximation is very good, but the more quickly the geometry changes, the less accurate it is.

 

[rob768]

If the stress-discontinuity is in an area of interest, re-define it, giving it a small fillet with high element density. If the area is not of interest, ignore it.

 

[AndyLake]

“Type of element is irrelevant.”
Yes, but the only reasonable way to model a complicated plate structure is model it by the shell elements. It is the time-consuming way to model the all fillets of the edges by using the shell elements when the structure is complicated. One means is to forget these stress peaks, but I should be known the right stress level when I make a fatigue analysis.

“would a non-linear analysis help ?”
The non-linear analysis is impossible in this case. The model has about 60 000 elements and the non-linear analysis demands much more elements, because the non-linear analysis expect a tight mesh.

“FEA will only give approximate stresses.”
I should be known the right stress level for the fatigue analysis.

“…giving it a small fillet with high element density.”
It takes a lot of time to model all fillets of the structure (for example, the corner of the several plates).

 

[johnhors]

Beginner77 - you use the type of element best suited to your model as a whole, which is quite irrelevant when it comes to modelling corners !

Unless you are constructing a mesh by hand (which I very much doubt), why should modelling fillets take a lot of time ?? What pre-procsssor are you using ?

"non-linear analysis expect a tight mesh" - Why ? Given the right hardware non-inear analysis of 60 000 elements is nothing extra-ordinary. Mesh is increased to accurately model rapid geometry changes - not for non-linear analyses.

"I should be known the right stress level for the fatigue analysis" - well one things for certain you ain't going to get any where near the correct stress levels unless you mesh your corner fillets accuately !

 

[AndyLake]

“Unless you are constructing a mesh by hand (which I very much doubt), why should modelling fillets take a lot of time ?? What pre-procsssor are you using ?"

- I construct almost all mesh by hand. I don’t usually use auto-mesh because of bad result (geometry of element is usually distorted). I use Femap 4.0.


"non-linear analysis expect a tight mesh - Why ?”

- Let’s imagine a model, which has 60 000 elements and size of one element is 20x20mm and thickness of 3mm. It’s totally impossible to get a correctly result because of too big element size. If you use too big element, the stress rises over the yield limit without plastic strain although the material is Elasto-Plastic.

 

[cbrn]

Hi,
in cases of stress concentrations due to discretization, the best you can do is:
- get the stress results along the edges concurring to the corner, starting from "sufficiently far" (what this means depends upon the model)
- plot the points "stress-vs-position", for ex. in Excel, excepting the point (corner) where the stress is manifestly "absurd", and get a trend-line of adequate order (for example, a parabola or a 3rd order polynomial)
- extrapolate the trend-line towards the coord of the corner: the value of this trend-line will give you a good estimation of the "real" peak stress.
- in case that the trend-line gives a result very similar to the value directly given by the FEM, then it should mean that the FEM value was already realistic (though NOT exact).

The advice to "small-fillet" the sharp edges is good, but not always practical (especially in very complex models with a lot of elements / DOFs).

Regards

 

[AndyLake]

Hi,

Thanks for the good advice!

Let’s imagine a structure which has two plates in 90 degrees. Then it is possible to get two different results (I can calculate the “edge stress” from two directions). On the other hand, should the result be the same regardless of calculating direction?


“…not always practical (especially in very complex models with a lot of elements / DOFs).”

- I agree. For example, it’s very difficult to model all fillets in the crossing point of the several square section beams.

Regards

 

[johnhors]

"Let’s imagine a structure which has two plates in 90 degrees. Then it is possible to get two different results (I can calculate the “edge stress” from two directions). On the other hand, should the result be the same regardless of calculating direction?"

You bet your life it should be !

Never heard of a "Free Body Diagram of Forces" ?

Hand calculated stresses should be the same regardless of whether you take forces and moments to the right or left of your section.

 

[AndyLake]

"Never heard of a "Free Body Diagram of Forces" ?"

- Never

 

[rb1957]

what, never ? (of course, the correct response is "well, hardly ever"; Gilbert and Sullivan)

but then i'm not sure how a free body diagram would help (determine the stress peak at a notch)

 

[AndyLake]

I know the free body diagram, of course. I have a small language problem and I assumed that Johnhors means ‘Freebody Display’ (in Femap). Sorry…