mesh convergence with stress concentration

[ygsygs]

Hello Everyone,

I am currently working on a linear static FEA with stress concentrations. I have not refined the mesh on the stress concentrations. The average stress in another region/surface without the stress concentration from 2mm-9mm mesh size has shown consistent output of about 30MPa, so i know the mesh setup has converged except on the stress concentration (represented by the max stress) which is showing a different behaviour. Trying to understand this behaviour.

My point of view is that, from 2mm - 5mm, the stress concentration is starting to be more pronounced and is growing exponentially in the results,
while from 5mm - 7mm, i believe this is a region where the stress concentration is not growing exponentially yet ( I can use results from this region),
while at 8mm and 9mm, (details below), I am not sure how to explain it.

Not included in this attaachment is: [mesh size(mm), max stress(Mpa)], [8,15713],[9,14552] which are way off.

Am I interpreting the results properly? What are your thoughts on the results?

 

[ygsygs]

rb1957 :

yes bad design to have the 90 degrees, and i definitely didnt take out a fillet out of there, the fillet is still there actually. its the way it was manufactured to have that 90 degrees effect. cant manufacture it directly but it can be a byproduct of the manufacturing process? an example of this area is : if you joined 2 rods of different diameters together with a circular weld, at this contact point if you put a small hole through it in such a way that each half of that hole is evenly on each ends of the rod, the center of this hole is at the circular weld. i think then you can have an infinite stress point at this area, because of the hole radius moving in all 3 dimensions, like a helix? well thats what the linear model seems to suggest. <-- hope this is clearer.

i cant really do anything much with the design. can only suggest, im not the product owner.

"a non-linear model will not predict an infinite stress at the root of the notch, because a non-linear is smart enough to realise that the the maximum stress in a part is ftu. a linear model is dumb, in that it'll extrapolate stresses beyond yield (and ftu)."
<--> understand. so elastic-plastic will show a non-convergence if the stress exceeds the ultimate tensile

"i'm not sure what your "cut-off" stress means in a linear model. and i really didn't "get" your reworded problem statement"
<--> when doing the linear modelling, i came across a trend as i refined the mesh: as i reduce the mesh, the max stress, initially converged, then about 3 or 4 refinements more it stayed about 5% difference from this converged value, i refined further, then it started to behave exponentially. so i took this converged zone as a "cut-off point" for my elastic-plastic analysis. not sure if this is ok but probably what i was doing was something similar to what stressebookllc says, i was taking an element or 2 away from the elements responsible for the infinite stress. but not sure if i can take a linear conclusion ( the stable/converged zone mesh size) and apply that mesh size to the plastic analysis. what do you think, generally the stress pattern would be the same on the component?


csk62 :

i think when defining the material property, the possion ratio is usually inserted in , so the iterations should be considering the possions ration effect? or would that be another setting in the modelling which needs to be activated?


stressebookllc :

"But this is not necessarily a bad thing. You can demonstrate that the high stress concentration area gets smaller and smaller with mesh refinement and you could consider the stresses an element or two away as more realistic. If you can indeed run an elasto-plastic material, then you will see there will be some plastic strain there. But the difference in the overall part deformation will show whether that plastic deformation is too much or acceptable. Especially for ductile materials (steel), it should be OK if the plastic strain there is less than a few percent. Because they are 'tough' meaning they can take load beyond yield and still not fail or fall apart on you depending on how much more load you apply"
<--> useful tips, thanks.

 

[rb1957]

"yes bad design to have the 90 degrees, and i definitely didnt take out a fillet out of there, the fillet is still there actually. its the way it was manufactured to have that 90 degrees effect. cant manufacture it directly but it can be a byproduct of the manufacturing process?" ... this is very confusing ...
1) is there a fillet rad in the real part ?
2) is there a fillet rad in your model ?

"i think then you can have an infinite stress point at this area," ... no, you can never Ever have an infinite stress; stress is finitely bound, a real number that can never be infinite. now the FEM might think it's infinite, 'cause FEM can be stupid. in a linear FEM, any stress above yield is fiction.

"so elastic-plastic will show a non-convergence if the stress exceeds the ultimate tensile" ... no, if the part is going to fail non-linear will tell you this 'cause it won't be able to apply 100% of the load. NL applies the load in increments, and if the last increment tried fails, then is says "oh, well; this is the last increment that worked ...".

another day in paradise, or is paradise one day closer ?

 

[Masse69]

ygsygs,

I too struggle from time to time with stress peaks above yield in linear models. It's probably self evident, but one should keep in mind that even if the FEA results can't be trusted at/near singularities (point load/constraints, reentrant corners), the stresses are high at those locations, and it is not good engineering practice to put features with sharp corners etc. in loaded areas of your design.

ASME provides the possibility to use linearized stress results, but I do not have enough experience/knowledge to say if the ASME methodology can be used for dimensioning in a general case. Neither have I seen/understood the justification for ASME's method.

IIW (international institute of welding) have developed techniques to handle hot spots at welds. These techniques are largely based on testing, are relatively easy to use but they are not always applicable in a more general case.

/Mats Lindqvist