Test results vs FEA results. 5

[kamal11]

We wanted to study the variation of a gusset/rib in a clamp. We tested a sample and it was bend out of shape for a load of 200lbs. I need to redesign the geometry to improve the load using FEA.
When i modelled the geometry , FEA has predicting the stress to cross the yeild stress at 10 lbs at one point. and the stresses in the neightbouring regions gradually decreased to value much lower than yeild strength.
In such a case what should be criteria on stresses to decide the load for making the clamp to bend.
Is it I need to take the section at the highest stress point and take that load that makes the least stress in the cross section cross the yeild stress. I want to make a decission based on linear static analyis only as i donot have stress strain for doing non linear anlysis
Regards
Kamalakar.

 

[kamal11]

The stress i talked above is not a stress due to singularity.

 

[GregLocock]

I'd almost give you a star, at long last somebody new is getting on the bandwagon - real world test results are very hard to duplicate in FEA.

Sadly I can't give you an answer, because I don't do stress analysis.

Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[GBor]

kamal11,

You will have trouble duplicating this test using purely linear, static analysis. As this object yields locally, the stress will redistribute. Linear stress will not properly redistribute the stress. If you look for "net section failure" (where the lowest stress across a section is yield), you will likely be conservative, but there is no guarantee.

You do describe

the yeild stress at 10 lbs at one point

If you refine the mesh in that area, does the stress level change much? Is the stress located at or very near a boundary condition? Is the yield point that you have in the model at or near the real-world yield point? There are many things that effect FEA results.

I have duplicated real world tests on many occassions...including non-linear situations. It isn't always easy, but it certainly isn't impossible.

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[corus]

I'm not sure why you need finite elements for this geometry. I assume that the gusset/rib is a T section. if you calculate the section properties then you can calculate the expected bending stresses by simple My/I, where y is the largest fibre distance. You may need FEA if the geometry is any more complicated and also to check local buckling of the part. If you're wanting to compare your FEA results with measured results then you'll need to use non-linear analysis methods if the section was permanently bent out of shape as you say. If you don't have the stress strain behaviour then simply use a bi-lienar curve with plasticity occuring at yield.

corus

 

[rb1957]

i agree wiith corus, i think FEA will be too difficult. i'd attack the problem from a different direction.

you know where the bracket failed (and where it didn't). why not add material where it failed (and remove material where it didn't, if you're picky about weight).

that, and a little (structural) commonsense should help.

btw, how much do you want it incease the strength of the part ? ... 10%, 100%. also, remember that this part is a component of a structure ... maybe strengthening this part might not be all you have to do (maybe the failure will migrate to the other parts of the structure). also, how well did the test fixture represent the rest of the structure ? maybe it was too stiff, causing the loadpaths to be not representative.

good luck !

 

[FEAHappy]

The first thing I would look at would be the displacement plot deformed. The animate it . Does the movement make sense? The displacement plot can show poor constraints.

Finite Element Analysis is faster and more accurate than handbook methods. CosmosWorks and SolidWorks are easy to use. However, there is a learning curve.

Finite Element analysis is accurate. However, assigning boundary conditions can cause incorrect results.

When in doubt, mesh fine. The only penalty is run time.

Your problem sounds simple. A FEA consultant might solve it for a reasonable cost. It is worth a quote.

Hope this helps.

 

[GregLocock]

Good grief.

"Finite Element Analysis is faster and more accurate than handbook methods"

Let's see, deflection of a cantilever. delta =W*L^3/(3*E*I).

I think we can assume that I'll have finished long before your FEA program has even launched.

"CosmosWorks and SolidWorks are easy to use." and like many easy to use tools are of limited use.

"Finite Element analysis is accurate." Yes, the solver accurately solves the problem you have set up. Whether that bears any resemblance to reality is another thing entirely.

"When in doubt, mesh fine. The only penalty is run time." No. The optimum mesh density is not infinite.

"Hope this helps. " well it made me grin.





Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[johnhors]

Well Greg, you did assume a uniform beam and ignored shear deformation, so you rather weighted the "contest" in your favour!

But yes you are quite right, the statement "When in doubt, mesh fine. The only penalty is run time." is rather scary ! Throwing zillions of elements at a problem, doesn't automatically improve a simulation, or magically correct poor boundary conditions as the words of the previous poster seemed to imply!

 

[johnsmith2]

How many people will do the convergence test on their meshing before they reach the conclusion that mesh is fine enough?

 

[GBor]

At least 1...

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[GBor]

Hey, Greg,

Let me say that I've respected your comments in the other areas where you've addressed questions, but if you

don't do stress analysis.

do you just lurk here to throw critical (not useful, just critical) comments out?

Garland

Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group

 

[bnrg]

I think that Gregg deserves a star for his post. I don't know the geometry of kamal11's hardware but a lot can be done without the reliance on FEA. Cheap FEA and PC's have only been around 15 years or so. We did accomplish many things before that.
I once asked a young ME how his analysis results compared to a hand calc estimate and he was dumb founded that anyone would even consider doing that. His professors (apparently anyway) never taught him to question the results. I don't believe in the old adage to question everything-I could never see how you could actually accomplish anything if you questioned everything-but FEA results need to be questioned.
Bob

 

[GBor]

PC based FEA started in 1980 and it is absolutely not perfect, but this is an FEA forum. Instead of acting like the tool is useless, let's foster an understanding of how to properly use the tool to simulate reality.

I'm all for hand-calcing, but some structures require a significant amount of simplification or an incredible amount of time to produce an answer that may suffer from many of the same problems found in FEA. I have a master's degree in structural analysis and love to analyze things, but I use FEA as a tool so that I can remain cost competitive. To date, nothing that I've designed using FEA has catastrophically failed, and tests tend to fall within 10% of my predictions.

I've seen many of those dumb-founded looks, but instead of criticizing the wearer, I prefer to educate them.

 

[GregLocock]

In FEA I do dynamic analysis, not stress analysis. Sometimes I do static deflections as well, but again, not stress analysis.

My background is that I worked in FEA for a few months, then switched to running a modal analysis lab, which is used to provide the FE guys with their primary correlation data. Since then I've worked in both fields off and on for 20 years. So, yes, I have seen many horrible things done with FEA, but /I/ don't do FEA stress analysis. Nowadays part of my job is to prepare the loads for static and dynamic strength analysis for components, but again, someone else creates and runs the models.


Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[gfbotha]

A few comments (in a thread that's already contentious!):

"CosmosWorks and SolidWorks are easy to use." and like many easy to use tools are of limited use.
Careful now... If a tool is made easier to use, it is not to say that it is not capable. However chances of potential misuse increase because of the broader user base. I solved non-linear (material) problems with similar software which e.g. NEi will only be capable to handle in its next release (results compared favourable with Abaqus results).

"How many people will do the convergence test on their meshing before they reach the conclusion that mesh is fine enough?"
I'll dare to say I don't do this every time. Simply because one does develop a feeling & experience and it also helps if you understand the particular element formulation. Because of many other assumptions I also don't hunt the 3rd decimal.

I agree with most of GBor's comments. And, yes, it is extremely important to ALWAYS do hand-calcs; at least as a sanity check!

Kamalakar, consider using a non-linear analysis with bi-linear material model (a la corus). Alternatively linear calculated max stress values can be reviewed (lowered) using approximate plastic correction as described in the book "Practical Stress Analysis in Engineering Design" by Blake. It involves hand-calcs and is an estimate only.

Cheers
Gert

 

[prost]

Doing a numerical convergence test should be as necessary and routine as the hand calcs, IMO. Each step, the hand calcs (which aren't just at the beginning of the analysis; I find hand calcs useful throughout an analysis) and the numerical convergence tests are important parts of the entire design and analysis process.

So add my '1' to Garland's '1' for a grand total of '2' who are admitting they do convergence checks every time. Of course I use a (h)p-version FEA code, and it's a lot more efficient and easier, not to mention one gets better convergence properties, than anyone using an h-version FEA code.

 

[prost]

Back to the original topic, one thing that always seems to hold me back is the lack of time to do a correlation of the experiment and analysis. The other major thing is lack of actual data, of course, which will always be a problem--you can never have enough detail in, say the photoelastic stress measurements, to make thorough correlation of the measured and analytical engineering data (strains, stresses, deflections).

 

[johnsmith2]

I ask the question to do the convergence checks. Because some of my co-workers don't do that, they decrease the element sizes as much as possible, and let the computer run for the few days (unnecessary computer cost), in order to ensure it is convergent.

 

[johnhors]

John,

"they decrease the element sizes as much as possible .... in order to ensure it is convergent" - sorry but unless you actually do a convergence test it is unsafe to assume that your mesh meets the criteria. This is especially true with auto-sizing routines which I have seen throw 100,000's of nodes and elements unnecessarily into low stress regions, but still leave critical areas with too coarse a mesh, despite the massive size of the whole model.

Prost,

Very often it is not possible to locate a strain guage on the exact point of interest as indicated by FE. Photoelastic measurements can also have their problems (depending on the method used) in critical regions. For these reasons we also locate strain guages away from any obvious stress raisers in what we call field stress areas to assist in validating our FE models.