Result Calibration Singularity
Result Calibration Singularity
(OP)
Hi folks,
This time I would like to ask about your opinion.
Below figure is self-explaining, you may notice 150 MPa applied to the tip of smaller solid object (lets assume it is mild steel) and below, larger box is providing supports. Assuming it is converged enough, in this simple example it is obvious real structure will "see" stress about 150 MPa in zone abutting to the larger object. But if the geometry would be more complicated, how would you be so sure how to get rid off this singularity? In other words, how to convince somebody that looking at stress range singularities are not real? I prefer to use stress linearization. What is your opinion? Please share.
This time I would like to ask about your opinion.
Below figure is self-explaining, you may notice 150 MPa applied to the tip of smaller solid object (lets assume it is mild steel) and below, larger box is providing supports. Assuming it is converged enough, in this simple example it is obvious real structure will "see" stress about 150 MPa in zone abutting to the larger object. But if the geometry would be more complicated, how would you be so sure how to get rid off this singularity? In other words, how to convince somebody that looking at stress range singularities are not real? I prefer to use stress linearization. What is your opinion? Please share.





RE: Result Calibration Singularity
TTFN (ta ta for now)
I can do absolutely anything. I'm an expert! https://www.youtube.com/watch?v=BKorP55Aqvg
FAQ731-376: Eng-Tips.com Forum Policies forum1529: Translation Assistance for Engineers
RE: Result Calibration Singularity
RE: Result Calibration Singularity
What is the material of the bottom? Have you tried to make it infinitely stiff?
TTFN (ta ta for now)
I can do absolutely anything. I'm an expert! https://www.youtube.com/watch?v=BKorP55Aqvg
FAQ731-376: Eng-Tips.com Forum Policies forum1529: Translation Assistance for Engineers
RE: Result Calibration Singularity
Did not make it stiff since it will not assist with answering my original question, and therefore it could not be applied for more sophisticated instances then.
Please look at this problem in this way: from strength of material you are 100% sure stress in the assembly will not be much above 150 MPa, but as FEA is a tool which brings in mathematical artefact in form of singularity, these singularities are "littering" true values and the question was how to explain this in professional way to someone. In my case, I think graph plots which are presenting immediate peak will explain why we may rid out of this values much above 150 MPa. How would you get rid off these singularities to report possibly accurate stress?
RE: Result Calibration Singularity
There's a modest stress peak in the corners. ok, may be real. certainly the assumption of constant 150 MPa = applied load over the same foot print is abit ... simple. It doesn't sound unreasonable to me that the reaction would be non-uniform, as the baseplate that isn't being compressed is behaving different to the part being compressed. particularly if you're looking at von mises stress ... maybe you've got tension and compression principal stresses ?
another day in paradise, or is paradise one day closer ?
RE: Result Calibration Singularity
RE: Result Calibration Singularity
Your Problem dissection-
1) There is abrupt change in cross section of the component at the junction of base plate as well as no smooth connection with fillets. This would be starting point of stress concentration.(Concentration Factor=235/150=1.5667). (This would change internal stress lines at the junction and concentrate these stress lines at this junction hence stress concentration)
2)If you assume the relative stiffness of the both bodies, the base plate stands out as more rigid candidate which is intensified by fix boundary conditions. This will resist the elongation of the connecting nodes of the members and you will see the high stresses in the connecting region.(The end face nodes will see more resistance and give singularity stress at the face itself if you have fixed the face of long member. Fixed face will now behave like rigid face)
3)In reality there will be high stress at these regions close to yield(sometimes crossing the yield)which is why if fatigue is expected as pointed out by corus, you cannot ignore these stresses. Anyway you should not ignore any peak stress blindly.
4)Stress linearization is good option to separate out peak from the average stress at this section. You can then find out from handbooks/theory/paper what is the stress concentration factor and compare your results with this and provide your client this calculation.
If you and the client knows the basics, you will find no difficulty in convincing about the stress singularities. But if not(mostly they act innocent
RE: Result Calibration Singularity
Cheers
Greg Locock
New here? Try reading these, they might help FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm?
RE: Result Calibration Singularity
I don't think it is a singularity att all.
You load the top part to have a stress of 150 MPa. Since the bottom part is larger the same load will result in smaller stresses/strains in that section. And that difference is more pronounced in the corners. That is because the stress will spread in two directions in the corners while it only spreads in one direction along the inner sides.
So the top part will experience the corners as stiffer supports and this results in higher stresses.
Is it clearer och just more confusing
Regards
Thomas
RE: Result Calibration Singularity
Since I do not have welds in the model, sharp corners (and stiffness at corners you all mentioned)are influencing load path.
In the same time convergence study shows as expected that those corners/edge values are hitting infinity and this is singularity.
So maybe I will ask you, were there instances in your experience that you included welds in your 3D FEA model too? Please note I am not asking about fatigue calculation.
I am curious what is your good practice.
Thanks for further responses. Appreciated.
RE: Result Calibration Singularity
I missread the problem because I thought the detail was in compression. On the other hand, if you don't use welds and the load path is the entire contact surface. Then there should be no difference.
You mention corner values that are infinite but your plot shows peak values of ~235 MPA with a load level of 150 MPa. What type of data does the figure show, exactly?
How have you postprocessed the data? First I would skip von Mises and use normal (vertical) stresses.
Regards
Thomas
RE: Result Calibration Singularity
235 is the cut off value manually input to adjust stress contours to be more visible, but normal stresses are much larger than 235 and goes up along with down sizing mesh.
Case is tensioned, not compressed.
At objects' edge, where the geometry change is made, normal stress nodal value consists of sum of: (A) Real 150 MPa of the applied force + (B) Real Concentration stress due to geometry change [would be visible if weld would be modelled precisely) + (C) Unreal Peak stress due to singularity.
The question is how do you estimate B and C in simple model I have proposed under consideration. Perhaps it is not achievable in practice without welds modelling.
RE: Result Calibration Singularity
RE: Result Calibration Singularity
My earlier post gives answer partly to your above question. You can use either stress linearization or average nodal/reaction forces at the point of interest as pointed out by corus also to get average stress which matters than singularity stress or stress concentration if no fatigue is expected.
Another thing I mentioned is you can get the stress concentration factors which may be available for some simple geometries and use it for comparing the stresses at the junctions. About peak stress due to singularity, you can check whether you have any modelling errors or analysis assumptions such as very sharp corners(I guess modelling the weld can minimize singularity stresses and you have more realistic stress), mesh sizes at the junction, contact non-linearity, altering boundary conditions(such as applying forces on the face or no of nodes rather than single node), Hertz contact stress etc. Altering all above factors may help in reducing the singularity stress.
RE: Result Calibration Singularity
Cheers
Greg Locock
New here? Try reading these, they might help FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm?
RE: Result Calibration Singularity
another day in paradise, or is paradise one day closer ?