linear and nonlinear analysis 1

[billy5]

Hi
I am new here and first i want to apologize on my bad english .
I`ve made a linear analysis for steam turbine blade(only centrifugal load is present) and when i have 28756 elements von mises stres is less then yield strenght (Re=550Mpa),but when i mesh model with about 50000 elements(refinament on the concentration area) vm stress reach almost 700Mpa(plasticity area)...i have to do non-linear analysis..which i`ve done,and vm stress is less then yield (550)...is this analysis acceptable?what does it mean?
Thanks!

 

[40818]

You probably need to give more detailed info about your model for any worthwhile responses. But basically your saying that if you increase the mesh density the stresses increase, have you continued to refine the area to see whether the stresses converge (level off)?
Give more details please.

 

[rb1957]

it looks like when you mesh refined around a stress peak, that the peak escalated ... not much of a surprise.

then when you allowed plasticity, the peak bluntened ... again not much of a surprise.

my concern, and i think 40818's, is if you're new to FE (or at least NL FE) you need to proceed with caution ... it's easy to be beguilded by a neat looking gui !

 

[40818]

yup.

 

[billy5]

Thanks for your replies.
Well i belive that any element have a minor error so if i have plenty of elelments that error multiplies so i get unreal result...is that correct? max von mises is on tooth peak in root(photo)..because of bondary condition on the edge is unreal max von mises?well i am aware that for FEA is very important experience which i don`t have ...how do i know which result is correct based on mesh density?
p.s. details about what,exactly?
Thanks again!

 

[cbrn]

Hi,
in addition to RB & 40818:
- two mesh sizes don't define if the problem is mesh-converged or not. The theory of FE will tell you that the stress calculation, especially for a H-elem formulation, is strongly dependent on mesh size, but will tend to converge at a "nearly-constant" value after a certain refinement has been reached. In order to be sure of that, you have to retrieve the stress always at the same location, progressively increasing the mesh density (decreasing elem size): plot stress vs elem size and solution time vs elem size; generally four runs can be sufficient to determine the optimal mesh size (optimal from a math point of view is infinite density, but this would also mean infinite solution time and infinite memory required, so you'll have to "cut off" at a reasonable compromise...)
- BUT, if you have a frank discontinuity (sharp edge, triple corner,...) then the above can't apply, and there are ways to demonstrate that the finer the mesh the higher the stress, without any convergence. In this case, either you modify the solid model by introducing a smooth (though small) transition, either you keep the mesh "acceptably coarse". What "acceptably coarse" mean is a bit difficult to determine, but a semi-empirical rule I've found is to set the elem size in the discontinuity zone at a value similar to the critical crack size in that location. Of course this requires more than one run, since in order to determine this you have to know the stress state... Ah, I forgot: third way is to build a very precise sub-model for the zone of stress concentration, introducing smooth transitions (small fillets, for example) everywhere.

- in a zone where you suppose the part to enter the plastic behaviour, it's no surprise that the stress "clips" to the yield stress, especially if you use a constitutive law where the plastic behaviour is... purely-plastic (Ep = 0). The strains there will grow up, though.

Regards

 

[rb1957]

first, yes there is an inherent error in FEA, but adding elements (reducing mesh size) reduces the error (rather than compunds it).

i looked at your picture ... what's causing the hot spot ? why is the first detail showing much higher stresses than the successive ones ? maybe a point load ? i don't know how you improved the mesh density (locally or globally, but i'd increase the mesh density locally (after i understood why the peak was there, and believed it was real)

 

[prost]

This numerical behavior you are seeing is most often due to a singularity of some sort in the exact solution, like a crack or a reentrant corner. If there is a singularity in the exact solution, then you cannot consider the maximum stress at the singularity to be meaningful. For instance, at a crack tip, the exact solution for the stress in infinity.

Looking at your picture proba1.jpg, it looks to me like a reentrant corner. Some might call it a 'kink' in the mesh. You have introduced a singularity in the mesh that is not there in real life--you would never build such a thing with this kink, right? In general there would be a fillet or the surfaces are smoothed out.

What kind of elements are you using? Linear (that is, 8 noded solids)? If so, then you cannot represent well a curved surface with as few linear elements as you are using.

 

[billy5]

Thanks for your replies!

I`ve used mesh with mixed elements (bricks and tetraedra) and let say that von mises stress exeeded yield (550 on 400°C)so i have to do nonlinear analysis..
What about nonlinear results? What can i find out from them and what is the max. strain which can be accebtable on this critical point?

 

[rb1957]

first, do you understnad the questions we've raised already ? before rushing into NL anlaysis, you have to understand what's creating the stress peak; critically, is it real or an artifice (fictional creation) of the model.

second, you question is very confusing ... if your allowable is yield then NL won't help ... NL detects when the material is stressed beyond the elastic limit and adjusts the local stiffness accordingly (allowing load to redistribute away from the yielded material). if yield is your allowable, then the part has failed (and a linear analysis is sufficient to show this).