Practical test methods for validating FEA and classical design calculations

[geesamand]

We have what is probably a common problem: we have a line of components that have been designed according to classical stress calculations (stress riser K factors, von mises calcs, etc). When we get beyond that envelope we use FEA. The problem is that when we use both methods to design a component that valid for both methods, we get a different result. The FEA results in a heavier/thicker component, presumably because the stress rises in corners and transitions that the classical stress checks ignore. Our FEA analysis have never been calibrated by real-world failure testing - the feedback is only real-world lack of failures.

Our components are designed for "infinite" life and in practice operate for decades in continuous service - therefore the classical methods are adequate and the FEA is conservative. The materials are ductile steel and stainless steels. Our stress limits are much less than yield point, to give you an idea.

How might we approach the question of making the two analysis methods more equivalent?

I was thinking maybe we can make test samples and (over)load them to the point of reaching yield? Then adjust the methods to ensure they calculate yield effectively, and from there, lower stress levels should also be consistent.

Thanks,

David

 

[acspain]

David,

Have you done a mesh study? To be clear, have you doubled and tripled the mesh densities and compared the results in identical locations between all three models (the third being your routine mesh density). I was surprised by the results the first time I did one.

 

[geesamand]

We use Mechanica (Creo Simulate) and that form of convergence has been confirmed but automagically by the computer as well as manually. I've also played around with local mesh size constraints and found the same kind of convergence.

I guess my point is we need to figure a way to set up stress limits or FEA practices that agree with the highly successful components that have been designed with classical methods. Perhaps we should establish a stress limit for areas where the classical calcs apply, and a higher stress limit for local stress concentrations. There is plenty of room between our normal stress limit and yield to do that.

 

[GregLocock]

One method is to use FEA to get the general stress levels but to then calculate the stresses at stress raisers manually.

Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376

http://eng-tips.com/market.cfm?

 

[corus]

The problem with classical methods of stress analysis is that they make many more assumptions about load paths and geometry than you would get from FEA that would take into account these secondary effects. Because of the 'hidden' assumptions in hand calculations, design limits (which are based upon hand calculations being used) are generally set low to take into account these unknowns. A comparison between classical methods and FEA are generally only valid in regions away from features where these secondary effects are less significant. You may also find that design fatigue limits are based upon nominal stresses away from stress concentration effects where FEA would show high stresses. These nominal stresses may be more in line with your hand calculation methods, but not necessarily so if there are secondary effects.

 

[geesamand]

There are certainly secondary effects (load interactions, stress risers). The classical analysis and stress limits have never produced a failure under well-understood loading.

I believe the problem is that we apply the same stress limits for FEA as we do for classical stress calculations. Are you suggesting that a fully-detailed FEA justifies a higher stress limit?

David

 

[stressebookllc]

I think the short answer here is that you do not want stress risers for infinite life anyway. Linear FEA will show you results based on the interpolation of the stress along the linear stress strain curve, so it is meaningless beyond the yield stress.

Refine the mesh there, use the actual stress strain curve, nonlinear static analysis.

If you can get mesh convergence within 1% to 3% of the previous value, then you will know the realistic zone of plastic strain there. If the plastic strain area is really localized and small, then you might use the stress levels 1 to 2 elements away as your amplitude to compare against your HCF limit.

Just my thoughts.

http://www.stressebook.com

Stressing Stresslessly!

 

[ShellsPlatesMeshes]

It is very difficult to provide a valuable advice without seeing an example with all the digits that you believe are unsatisfactory. With the FEA there are many factors involved influencing the quality of numerical results.

 

[rb1957]

"How might we approach the question of making the two analysis methods more equivalent?"

well, you've got a classically designed component that has worked well (not failed). therefore an FEA of this component, whatever it shows, is acceptable; no?

of course, you started your problem statement with "When we get beyond that envelope (supported by classical calcs) we use FEA", so how do you compare the FEA of a new part with this FEA of an existing part ? maybe ...
1) the highest stress on the new component is no higher than that demonstrated on the existing part ? (but this might bring mesh sensitivity into the discussion)
2) compare the amount of the structures at "elevated" stresses ? (how localized are the stress peaks)

3) maybe stick to doing classical calcs ? but you'll probably bump into customers wanting FEA !

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

 

[geesamand]

Yes, I know I'm not showing the details of an example and due to the proprietary (and obvious nature) of the data I cannot do so.

I had considered performing a few well-converged FEA's of designs considered "good" that were originally based on classical calcs, to see if there was any consistent limit to stresses or areas of stress concentration.

We use FEA where classical calcs become very difficult to apply. Where the joints are simple in cross-section we are fine but we have better optimized section shapes that do not lend well to classical analysis. And yes, a few customers want FEA.

David

 

[trainguy]

One method many people use is to validate your FE model by doing a static test, with strain gauges appropriately placed. I would use non-linear materials, to be ensure your hotter spots behave as per real life. Compare the measured stress distribution with that obtained by classical calcs.

Then, use your measured stresses in a fatigue calculation, paying close attention to selecting proper fatigue details that do not effectively stack-up safety factors.

The advantage here is that your fatigue calc is not dependant on the accuracy of your FE model.

tg

 

[geesamand]

Good thought - I had forgotten about the possibility of strain gauging near / at the stress riser locations.

Fortunately this is not a reversing fatigue loading situation. Life here is 30-50 years of continuous service as a rotating machine, which is "infinite" compared to any low-cycle or even high-cycle fatigue example.

 

[rb1957]

btw, it's very hard for s/gauges to pick up the stress peak. s/gauges are better used to measure the "bulk" stress, away from stress peaks to validate the model.

if testing, just static test (to ultimate) to show it good.

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

 

[harishbm]

Hi
Geesamand

FEM tools(Ansys,Nastran) are developed based on classical theory. You can check this with simple cantilever beam with concentrated load at its free end. Your results will match 99.99% with the theoretical calculations. But for the larger models FEM is a better option. Because there are no standard formulae are readily availabe. In calssical approach calculations are done based on considering factors like notch radius, key way compliance etc. For big and complicated model it is very tough to bring in exact geometry of podcut for calculation purpose.

With a good practice in FE modeling and Analysis you will get best results with a little variation of 8-10% of the theoretical value.

More over with FEA you can easily change your design criteria like topology,material,structure strengthening etc.
All this can easily done ,which results in quicker product life cycle.

There are many FEM tools are available like : Nastran, Ansys, LS dyna