Strain Gage Analysis versus FEA

[feajob]

Hi,

We have to do some static tests on 3D parts and correlates the obtained results with those obtained by our Finite Element Models. The question naturally arose, how do we know where are the best locations for strain gages installation?

I believe that due to the limitation in strain gages installation, we cannot put them in sharp corners. So, in order to find out the best locations, I checked the hot spots due to the FEM Maximum and Minimum principal 3D stress distributions for each test load condition. I believe that presence of a single or multiple load path at FEM spot suggests using strain gages with linear or rosette pattern, respectively.

I know that correlation between test and FEA is not an easy task. For example, following items may have impact on this job:

o Residual internal stress from manufacturing;
o Difference between real material properties and test alloy;
o Loading the part beyond the elastic limit at any location on the part;
o Complex imperfect 3D geometry;
o Strain gages not calibrated perfectly;
o Insufficient mesh density;

I would like to know about your experience with the Strain Gage Analysis versus FEA. How do you decide about the best location (and type) of strain gages on your 3D part?

Thanks,
A.A.Y.

 

[rb1957]

generally keep them well away from "spurious" stress gradients.

correct the s/g output for everything under the sun (obtain accurate material properties from coupon tests of the same batch of material, etc)

be really happy if you're anywhere near 10% different from the FEM

what you may want to do, if the results are completely different, is to strain aguage the interface of the detail part (ie, get the loads coming into/out of the part).

finally, good luck (you'll need lots !)

 

[rstupplebeen]

Your strain gage manufacturer should be able to help with selection based on materials, temperatures, loading conditions etc. As far as location that's predominately up to engineering judgment. Stay away from areas with large strain gradient because it will be location sensitive. Avoid difficult areas to place them. Remember the strain gage is basically reporting the average strain under the gage section. Determine what % correlation you are aiming for before testing. In some industries 10% is great in others 1% is unacceptable. If you don't get buy in early people will always say well the model has errors. Good luck.

Rob Stupplebeen

 

[feajob]

rstupplebeen, it is a good point, I understood that I should avoid large strain gradient, but not necessary large strain region as long as they are less than elastic limit.

rb1957, I am not quite sure if you are referring to the large strain gradient by using spurious stress gradient or you are pointing to another issue. I am agreeing with you, I need to have good luck to get acceptable level of correlation between test and FEM results. I believe that 10% is an optimistic number. I will be happy even with 25%.

A.A.Y.

 

[gwolf2]

feadude,

I´ve done a lot of this. It´s easier than you think. With metal components, well chosen and accurately positioned gauges you should have no problem with getting well under 10%

I think the previous posts have covered all of the salient points, making me wonder what more to add............

It´s this - make sure that the boundary conditions in your model REALLY match reality. Check the hardware setup and fit. On complex jigs, make sure that the test hardware stiffness assumptions match your model assumptions and if necessary even model the test hardware.

Have fun!

Gwolf

 

[gwolf2]

Sorry, Feajob, not dude, Feadude is another poster I think.

 

[GregLocock]

Good on you for correlating your model. Even if the results are awful at first you will learn a lot. Have you done a modal correlation first?




Cheers

Greg Locock

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

 

[BobM3]

Addressing some of your concerns:

1) Residual stress won't show up on the gage. Attach the gage when the part is not loaded. The part may have a residual stress at that point but the gage will be at zero strain.

2) Gages can be calibrated fairly accurately, certainly within a percent or two. It will be one of the smaller errors overall.

 

[gurmeet2003]

I have done some strain gage testing for model validation. However my results have not been as good as those reported by some members above. 1% agreement for any model appears to be very optimistic. Usually getting mesh convergence within 1% is not easy.

Most of my models have bolted joints. There is alwyas some uncertainty in loads. Also quite a few models are assemblies. If I get results near 20% I consider them good.

High strains usually occur near areas of high strain gradients. Therefore significant diffrence in results would occur due to placement error at these locations. Strain gage calibration error would be negligible in comparision.

The sources of error could be as follows:
1. Uncertainty in material properties
2. Uncertainty in load
3. Discretization error which can be established by mesh convergence
4. Uncertainty in geometry
5. Uncertainty in boundary conditions
6. Uncertainties in test conditions

Difference between analysis results and test results is subject to all of above. To get good agreement significant effort in reducing all of the above uncertainties is required. I think it would be difficult to get an agreement of 10% based on a single test.

Gurmeet

 

[GregLocock]

I know a lot of test engineers that think that it is important to put the strain gauge near a failure point, whereas for FEA correlation your biggest problems are more likely to be in estimating the loads, and boundary conditions, so a high strain point is not automatically the most valuable location.

Cheers

Greg Locock

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

 

[joesm519]

I do this type of comparison all the time and I have found the results to be with in 5% and sometimes with in 1%. I think the trick is not so much in the FEA but in the strain gaging. Make sure your placement is very PRECISE in terms of location and direction of the grid.
HTH

 

[feajob]

BobM3, this is a good point about residual stress.

gurmeet2003, you have described very well source of errors. As I mentioned previously, I think that 10% is a fair agreement. If you don't mind, could you share more details about your experience? What was the percentage of agreement for your structure? What kind of structure are you dealing with?

GregLocock, You are right, our main purpose is to validate the load paths and correlate essentially our stick model (3D Beam Model) with real assembly. However, we will try to validate our 3D detailed FEM Models (meshed with tet 10 elements) at the same time.

joesm519, It's good to find that your test results are with in 1% to 5%. I am wondering if you can share more details with us. Could you please give us more detail about the type of structure you are testing?

FYI, I am dealing with a 3D Assembly Aeronautic structures.

Thanks,
A.A.Y.

 

[rob768]

residual stress will not show in your real world model, but also not in you computer model (unless you model is as a load case). As long as no plastic deformation occurs, disturbing the correlation between calculated elastic stress and real world behavior, you will ok.

 

[joesm519]

feajob,
The parts I design, analyze and calibrate are wind tunnel force tranducers. The analysis is done on a part while the calibration is done with a assembly. The transducers have multiple load paths and have forces and moments applied in multiple directions. The material is typically steel or aluminum. We also strain gage composite panels which we don't calibrate.
HTH

 

[gurmeet2003]

FEAjob,

Usually models I deal with are complex shaped casting assemblies including 20-30 bolts (recip compressor parts). Bolt preloads are important. The strain gage locations are on the inside and not easily accessible. Gaskets are also involved.

Gurmeet