Hello,

When you have a stress singularity in a part and you see that the stress is totally irrelevant how can you then find

the highest occurring stress in that part?

thx,

Theo

Hello,

When you have a stress singularity in a part and you see that the stress is totally irrelevant how can you then find

the highest occurring stress in that part?

thx,

Theo

Here's one method:

-Use the 'Split' feature to make separate bodies in the singularity region

-Make sure the new split bodies are appropriately bonded to everything else

-Make sure boundary conditions are still appropriately defined

-Run the study

-Either hide the bodies, then view the results plot - or - advanced / show plot only on selected entities

-Under chart options 'show min/max range on shown parts only'

Adding split lines to create new faces and splitting bodies into separate pieces are both important skills for analysis. It seems like a little extra work, but it's often necessary to help get the exact results plots and charts or visualization you need.

The long answer depends very much on where you got your allowables (specifically, how the stress in the allowable is defined), what is causing the stress singularity, whether there is a fatigue issue, and whether the singularity is a pure modeling artifact or is closely related to a stress concentration in the geometry, among other things. Can you send a few screen shots? Rarely is the globally computed max stress going to be the driving quantity.

The short answer, though, is judgment. For instance, yielding is occurring through less than 5% of the section, this is strength (not fatigue), and outside of the concentration the stress is low, so call it a pass.

Hi,

I attached some pictures. I did an H adaptive study and no convergence message after 5 loops. When I plotted the convergence graph i got picture 01.jpg, so you can see convergence on displacement but not on von Mises stress. In picture02 you can see a max.Von Mises of 28000 N/mm2 !! so totally crazy.

Looking deeper in the plots i used an ISO Clipping (picture03) with a value of 690 N/mm2 (the yield of 31CrV3 with a factor of safety of 1.5) and two small areas were found where sharp edges are in

contact with the faces (both parts are made of the same material)

Picture04 shows where the stress is situated and 05 and 06 are the parts involved.

For me this is clear, no problem, but a colleague wants to know what the highest stress is in that part.

Displacement converging while stress diverges is normal. For H-adaptive, a better convergence criterion is strain energy, which will converge around a singularity even while the stress diverges.

If you model an interior corner, you will see a stress singularity. If this is not fatigue, you can go out about 3 elements and take that stress as the nominal. The stress in the corner will be relieved by local yielding, so what you want to show is that the volume of local yielding is low as a percentage of the cross section.

With respect to strain energy, you have to choose the convergence criteria, is my recollection. I haven't used SW simulation in years.

Not exactly St. Venant's. The assumption is that if material yields in a very small area, it will flow to redistribute the stress and then yielding will stop. This assumes that there is enough unyielding material to react the load without the elastic behavior changing very much. If a large percent of the cross-section is yielding, the linear model becomes very inaccurate because the elastic behavior does change, but the model ignores it.

But 1% is very small. If this is not fatigue, it's going to be fine. But if it is fatigue, over many cycles the very small local yielding can lead to cracks which can propagate and compromise the structure. So for fatigue you would have to dig much deeper into this. Also, this is a bad design for fatigue. You have to design out stress concentrations for cyclically-loaded parts.

Keep in mind that you've modeled a perfectly sharp interior corner. This is impossible. But if it were possible, the stress would actually be infinite. So the divergent result is accurate and correct, given what you've fed into the model. In real life, there is some finite radius. Even if you machine it sharp, end-mills have approximately .0002 radii on the corners. So the stress will technically be very high, but not infinite, and the material will flow and relieve it.

If you don't need the sharp geometry, fillet that corner and re-run, and you will rapidly see that everything is fine.

Theo, may not be the most slick way of doing things, but if you right click the stress plot and use ISO Clipping and start the slider bar from the far right hand side, you can drag left and you will see the elements of the model that are taking on the highest stress- the singularity will come up first but then more of the model will begin to come into view. At that point you would have a good idea of the regions, and also on the legend, it will show the stress value being observed at that time (black arrow)- then on an unclipped result plot I guess you could change the upper limit of the legend to the more realistic peak stress that ISO Clipping gave. Otherwise i guess eliminating the singularity with a more refined mesh, or if a sharp internal corner, rounding with a radius.