Stress Concentration Factors and FEM

[jdps]

I have been playing around with the idea of deriving stress concentration factors from finite element models and have some questions.

I have a simple model of a plate with a hole with an axial load applied. As I refine the mesh near the hole, the stress concentration factor I derive from my FEM model converge to what it should be (according to Roark). This works for simple geometries with simple loading.

Continuing with the plate with the problem of plate with a hole under axial loading:
My understanding is that as the loading increase, the stress near the hole will increase till it eventually exceeds the materials elastic limit. At that point, local plastic yielding occurs and the stresses near the hole remain constant while the stresses at a distance increase. This happens until the entire width of the plate is yielding and failure occurs. I believe that standard static analysis relies on this form of failure in that it doesnt account for stress concentration factors. It simply takes the axial load applied and divides by the effective area. This should work only for somewhat ductile materials as they should follow the failure process i described above.

My questions are the following:
- Finite element analysis accounts for stress concentration factors with the model geometry. Would it be theoretically correct for me to take the stress at stress concentrator locations and divide by the stress concentration factor? This would be equivalent to standard static analysis that i described above. This would assume simple geometries with known stress concentration factors that have simple loading with stresses that have converged. Im assuming theres no way to apply this to complex geometries with complex loading as there would be no way to determine what the stress concentration factor should be.

- Can you think of any papers or studies that detail how the stress concentration factors derived from a FEM converge as the mesh is refined? Or how this could be applied (or not) to more complex geometries with complex loading?

 

[rb1957]

"Would it be theoretically correct for me to take the stress at stress concentrator locations and divide by the stress concentration factor?" … why ? for what purpose ?

Do you want the nominal stress on the section ? use an element some distance from the concentration, or take a cross section and average the stress. But why do you want this ?

It would be somewhat reasonable to say the the stress peak in a linear model is exaggerated at the stress concentration, that yielding would blunt this stress. And that this yielding would not be significant … unless of course it is … like leading to yield of an entire loadpath (development of a plastic hinge).

"This would be equivalent to standard static analysis that i described above." You are correct in that static analysis (usually) ignores local stress concentrations and would react the load over the net section (calculate section properties based on area, determine local loads, calculate stress). If you want to do anything with your FEA you could extract the local loads over a section.

I think I've done something similar … I had a complicated fttg to analyze, did FEA on it, static analysis peachy (a little local yielding, NBD. But for fatigue I looked at the stress peak, said the peak stress is about 1.5 times the nearby stress, so Kt = 1.5 and went off t o find an s/N diagram.

"Can you think of any papers or studies that detail how the stress concentration factors derived from a FEM converge as the mesh is refined?" As you've done … fine tune the FEM until it agrees with handbook solutions. I use Petersen "stress concentration factors" as a specialised source of Kts … Roark is a bit of a jack of all trades.

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

 

[SWComposites]

Thousands of papers have been published on stress concentrations and FEA. Use scholar.google.com to search.

FEA does not “account” for stress concentrations. It approximates them. Sometimes closely. Sometimes very inaccurately.

 

[jdps]

"Would it be theoretically correct for me to take the stress at stress concentrator locations and divide by the stress concentration factor?" … why ? for what purpose ?

Say I have a fitting with complex geometry and complex loading, I am trying to determine if there is a valid method to determine the stress concentration factor at say a fillet on the fitting. That way i could theoretically divide my max stress on that fillet and potentially show a positive margin for static analysis. I do not believe this is possible to do as determining the stress concentration factor for a complex geometry with complex loading would likely be impossible or at least require a lot of testing. I would also have to have a much more refined mesh. So while theoretically possible and correct, I do not think its a valid method for analysis. Am i correct?

Thank you for the suggestion to use scholar.google.com, I will try and find some papers on the topic.

 

[rb1957]

"I think I've done something similar … I had a complicated fttg to analyze, did FEA on it, static analysis peaky (a little local yielding, NBD). But for fatigue I looked at the stress peak, said the peak stress is about 1.5 times the nearby stress, so Kt = 1.5 and went off to find an s/N diagram."

I wouldn't use stress concentration factors for static analysis (in part for the reasons you've explained … too local). To analyze a complicated fitting with complicated loading, I'd use the FEM stress. Possibly the number from linear FEA is too high … run NL FEA or explain it away as insignificant local yielding. Possibly work some mathematical witchcraft with neuber's analysis. The FEA will tell you if the whole loadpath is "failing" (which is a bad thing and will need redesign) or if it is "just" some localised stress peak (which should be ok).

If "hand waving" it away doesn't work for you, then run NL FEA and get something closer to "truth".

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

 

[SWComposites]

OP, you are correct for complex fitting. You have 3 options:
- throw away the FEA code and analyze the fitting using classical hand analysis methods that were used for decades.
- size the fitting to the peak stress values from the linear FEA and accept the weight.
- run a material nonlinear FEA using actual material stress-strain curve, and write static margins to ultimate strain. If you do this you should also run a linear FEA at fatigue loads and check the peak stresses vs yield stress.