Reporting Max Stress

[ahad29]

Is there a rule of thumb in reporting the max stress on a part on which FEA is performed using a p-element FEA softfware like pro mechanica. Sometimes the max stress occurs on a stress concentration area where the max strtess reported in the legend is very high and occurs on a point or a very small area. To make things worse the solution does not converge at that location. In such cases what do you consider your max stress is on the model.

ahad

 

[chris9]

Ahad,

You've got to decide which stress values are spurious and which are real. I only report real stress values. If you're not sure whether or not the stress is real or spurious then you should carry out convergence checks.
Usually large differences in stress between unaveraged and averaged elements means it could be a singularity or that it is not fully converged.

 

[corus]

You don't tend to report the maximum stress but report on stresses everywhere in a structure as each may have different limits to satisfy.
A high stress at a point will occur because you have applied a point restraint or point load. If you haven't or can't otherwise justify this high stress then you've most likely made an error.

corus

 

[ahad29]

Thanks corus and chris9.
Corus, I do not have point loads or point restraints in my model. Sometimes the high stress in my models is right at the edge of a rectangular beam or at the intersection of two orthognal radii which forms a curve. This clearly is a case of stress singularity, which i confirmed through convergence runs. The red area which is the highest stress is vey small almost say 1/10 the size of the element itself (ofcourse with p-elements the elements could turn out to be of any size, I mentioned this only to explain that the region is very small). Therefore I was wondering if there is a guideline or a rule of thumb that says the stress in that region is that which corresponds to the color which covers atleast a couple of elements and not just a very small part of an element. Hope my question is worded clearly. Thanks.

ahad

 

[corus]

You need to know about design analysis and the classification of stresses. The classification of a stress should have nothing to do with the element size which are purely the means by which you calculate the stresses. Read a design standard such as the Pressrue Vessel code which has a good description of how to assess and classify stresses in a structure (not just vessels). At a stress concentration you'd class the stress as a peak stress, which contributes to fatigue damage and would be assessed that way.

corus

 

[chris9]

Ahad,

You've already identified the stress as a singularity so ignore it. If you're worried about what the real stress is in that area you could alter your model to remove the singularity.

 

[ahad29]

chris9,
Could you give me some tips as to how to alter the model to remove singularity. Thanks.

 

[chris9]

Mixing elements (beam/solid/shell) sometimes cause singularities at the join. You could try meshing just in solids. Also bad geometry (overlapping surfaces etc) cause singularities. Look for faults in the surface geometry and correct it. Restraints and loads in the immediate area of interest could also make the results spurious.

 

[corus]

A singularity will occur at a right angle formed by two sections. In reality there will be some kind of fillet radius there or a weld. Unless you were concerned about fatigue then you should plot the stress distribution up to the singularity and from the distribution estimate the stress if the singularity was not there. This stress at the structural discontinuity will be classed as primary plus secondary with a limit of twice yield.

corus

 

[ahad29]

chris9,
My model has all solid elements but the load-case is such that one of the sharp corners of a rectangular beam is seeing this high stress due to singularity. To be more precise the high stress is on the curve that forms as a result of two radii intersecting at the foot of a rectangular beam. I am not sure how singularity in this area can be overcome. Thanks

ahad

 

[MToft]

Hi,
Are the two radii the same? It might be possible to improve the understanding of what's happening by changing the rads (while keeping them the same as each other). Also, if possible, maybe review the convergence performance, error estimates etc to see what the solver's own estimate of the "real" stress looks like.
Are the two radii blended into each other (more "real") or is there a sharp edge? If sharp then maybe try blending them (filletting the fillets!)
Good luck...
MToft

 

[ahad29]

corus,
I plotted the stresses and I do not see any abnormal spikes. And also I ran another "MPA" with higher order polynomial (7) the convergence % has reduced since the last run which used a polynomial order of 6. I guess this shows that there is no singularity. I have six loads and below are the error % and convergence % for the polynomial order of 6 and 7
=================================================
P=6
Error %==> 2.3 3.2 2.5 3.0 2.0 2.2

p=7
Error %==> 1.9 2.6 1.8 2.3 1.4 1.6
=================================================
p=6
Convergence% ==> .4 7.5 1.7 1.6 9.3 10.8

p=7
Convergence% ==> 2.8 4.0 0.9 0.1 0.0 2.9
=================================================

Does a reduction in %error and %convergence from P=6 to P=7 necessarily mean that there is no singularity ? If yes then from the results above it means there is no singularity in the model. The change is the convergence has changed the Von Mises stress in the following % from P=6 to P=7
Delta Von Mises==> 2.7% 3.9% -0.7% 0.1% 0.4% -2.9%

MToft,
The radii are of the same size. the way the radii are machined and upon closer observation it doesn't look like there is a fillet on top of the fillet. I could assume a .001-.005" radius at the most but from previous experience I have seen that Pro/Mechanica does not discretize the model as if there were a fillet that small in that region.

I greatly appreciate your suggestions. Thanks

ahad

 

[corus]

If you're reporting a high stress at a point then that must be a spike when you plot out the results. Try looking at a picture of your stress results rather than the numbers that are printed out so that you can make a valued judgement of your results in relation to where they are on the model.

corus