FEA Model versus Actual Results
FEA Model versus Actual Results
(OP)
I have modeled several simple metal cantilever beams in Algor and have compared the results to actual Instron pull (push) test data. I have applied a small displacement at one end. The models calculated force is always 30 – 50% higher than actuals. The FEA results agree with the hand calculated force using formulas from the Machinists Handbook. Any suggestions?





RE: FEA Model versus Actual Results
If you are using beam elements for your FEA answer, this would be expected to match well with theoretical calculations. However, if your actual part is sufficient short in its length, beam theory may not be appropriate.
Other possibilities could be nonlinearity, or differences in effective boundary conditions.
If you put small displacements on the cantilever tip, does it respond linearly? Be sure to compare this initial response against you theoretical/FEA responses, as this initial response SHOULD be linear. When the F vs d curve starts diverging from linear, your linear assumption for your analytical models no longer holds.
Also, look into recommended ratios for beam length vs height/Ixx. Beyond a certain ratio, beam theory does not adequately describe the actual behavior of the beam.
Brad
RE: FEA Model versus Actual Results
The beams are not short. I used several very different geometries. One example, C260 brass is t=0.82mm, w=19mm, l=27mm and small displacements d=1 mm or less. In this case the force displacement curve is linear until 1.8mm. I always stay well within the linear range.
Thanks,
Bob (rpm63)
RE: FEA Model versus Actual Results
I think of two possible reasons:
1). Boundary conditions. Is it your experimental model completely fixed? Rotation of the base could produce additional displacements.
2). In your FEM model, if you are using 2 or 3D bricks (linear elements), you could have shear-locking. This happends when beams (shells) are modeled with low order elements (low order elements are to stiff to represent bending). To fix this, you need to use more elements through the depth of the beam or use either cuadratic or cubic brick elements. Alternatively, you may use linear elements but with 'enhanced modes' or elements with 'hourglass' control.
cmfg
RE: FEA Model versus Actual Results
I am not using beams/shells. Also I have gone as high as 8 elements thick and the FEA answer does not vary much.
Thanks,
RPM63
RE: FEA Model versus Actual Results
What kind of elements are you using?
RE: FEA Model versus Actual Results
Are you using the correct E value ?
Are you applying a point load or a line load? (The beam is wide and could be deflecting as a plate rather than a beam, with addional transverse deformation).
Are you clamping it adequately ? (This was mentioned by Cmfg as well).
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
I have used several standard materials with published E values, (brass and steels). Could they all be this far off? I get my E values from Matweb.com, texts, and other sources and they all are about the same for each material. I have suspected this but have no way of varifing this in-house. I would have to pay to have a lab test the material. Even if I have it tested, this would be an average E, what if the material is not isotropic because of colled rolling etc. If I have to have a material tested before I use it, it kind of defeats the cost savings of FEA.
I am clamping the test specimen pretty good. I also suspected this could be the problem so I created a simply supported test along with a FEA model. Same thing, FEA results 30-50% higher.
I am using a point load for and the model and test. The test specimen gets contacted with a thin blunt tip object so it does not penetrate into the specimen and I am pushing it down. For the model, I am applying a displacement on one node.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
You state that the model's force is higher than that of the actual test, therefore the model is effectively behaving as stiffer than the actual test.
I would explore some of English Muffin's ideas. This really does appear to be an issue of your test not being consistent with the assumptions employed in your beam/FEA models.
Specifically focus on answering this question: What could make the tested configuration more compliant than my assumptions account presume?
As EM suggests, instrumentation could be off. Another thought--is your test fixture effectively rigid compared with your test specimen? One of my buddies jokingly refers to "Fixturing" as "The F-word of test-to-experiment correlation", as failing to account for fixturing compliance can lead to significant errors. Just a thought.
An interesting problem. Keep throwing out more info.
Brad
RE: FEA Model versus Actual Results
Have either of you done a similar bending test and come up with accurate FEA results vs. actual measurements?
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
It sounds like you have enough test data to back calculate values for E (Youngs Modulus) for the beam test setup. This will almost surely give a value different from that you are using for the FEA computations....A second step would then be to take one of the beams and do a simple tension test and determine the value of E from this....Comparison of these values should give you a better idea of whether the difference is comming from bad material property values, boundary conditions or some other condition...
EdR
RE: FEA Model versus Actual Results
The tension test will certainly confirm whether E is correct.
I will second EnglishMuffin's experience. I have done such comparisons multiple times. This should be able to readily correlate.
Brad
RE: FEA Model versus Actual Results
Did you try with different number of elements as well as different order of elements to see if the result converged to some value? If that is not the problem, to my mind, the three possible reasons behind this could be: (i) inaccurate material properties, (ii) inaccurate simulation of test boundary conditions and (iii) inaccurate simulation of test load. If all these are satisfied, your result should be within 1-2% of measured value.
Sudip
RE: FEA Model versus Actual Results
This is easy to measure accurately, in practice. Once this is correlated then you can look at boundary conditions.
Cheers
Greg Locock
RE: FEA Model versus Actual Results
Verification of E value from tensile testing may not be correct because of testing machine compliance considerations. I think it should be verified with some accoustic measurements (Please educate if I am wrong).
Another thought is that "Is the mesh used in the FEA is optimum, i.e. whether a mesh sensitivity analysis was done before comparing the results with experiments?"
Utpal Borah
RE: FEA Model versus Actual Results
rpm63 says his (ok, so there's a maybe 1% chance of him being a her...apols if so!) FEA and hand calcs agree, which implies that shear deflection is not significant, and that there's no major problem with the FEA. rpm63: could we possibly ask for the formulae you used for finding the force for a given deflection?? (Along with the E values, etc.)
[If shear deflection is turned off for the beams and shells this would make the analysis over-stiff compared with reality, as observed. However, the solid element models should shear correctly, and anyway, the shell element calcs would normally have shear in.]
I would be astonished if E was even 20% wrong, let alone 30%-50%! Some titaniums can vary by maybe 10% from published values, but most materials are pretty reliable for elastic stiffness. The small deflections rpm63 is imposing don't look as if they could possibly be yielding the materials mentioned (which would also cause real forces to be below analysis). rpm63: what is the max stress calculated in the beams??
The use of both a simply supported and cantilever geometry should at least show a difference in results if fixturing is defective (which it "fixturing" well could be, even for such a simple set up).
Given all this I would tend to suspect the test setup, though it does seem like the easy way out. rpm63: how are you recording deflection? If you are using crosshead travel, this can be significantly in error for small initial movements (depends on machine a lot). Using an ordinary dial gauge or even a simple scale on the part might be a prudent check (apologies if this obvious and you've done all this stuff).
Please don't let this one die off...this sort of discrepancy between reality and analysis can be very enlightening, as well as intriguing and fun.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
I think you actually mean "nonlinear geometry" or "finite rotation", which has already been ruled out. If finite rotation is an issue, then it should not be behaving with a linear response. The poster has already stated that the initial response is linear.
rpm63--as suggested above, please follow-up with additional information. These types of problems are really fun, and are what help to make better FEA engineers out of all of us.
Regards,
Brad
RE: FEA Model versus Actual Results
Yes analysis should linear with reasons stated before.
I verified my measurement instrument. I was using Instron pull tester. I re-measured using a completely different piece of equipment and got similar results.
Here are some numbers. Cantilever beam 1.08 inches long x 0.75 wide x .032 thick. C260 brass ½ hard, E=16,000,000 psi. At deflection (d) = 0.040 F (measured) = 2.4lbs. FEA results yield F= 3.1 lbs when applying a -0.040 inch displacement to the end. Therefore, 30% off.
Hand calculation equation matches FEA exactly: I=bd^3/12, d=FL^3/3EI.
Stress stain curve is linear until 0.071 inches.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
I shouldn’t have used the term exactly. The hand calculations were 7% different. I was only using 2 significant figures and converting from metric to English, close enough for me. I would be extremely happy to be within 10%.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
The force measurement could easily be in error depending what you are using to measure it. A typical load cell might have 0.1% accuracy, so a 5000 lb capacity load cell is only accurate to +/- 5lb. What are the specs on the Instron?
You mentioned measuring with other equipment, like what? For something like this dead weights and a dial indicator would be a good sanity check. If it matches the bending I agree with the others, do a pull test on your Instron for E.
EnglishMuffin, though it doesn't sound like a modeling issue please explain the bit about point load vs line load. Are you talking local deflection at that node? I wouldn't expect it to matter much here due to the low force. But if you take the average deflection of the end nodes line and point results should match, right? But it's an important point in general that deflection at the node of applied force is higher than reality.
RE: FEA Model versus Actual Results
I have started some checks on modelling some blocks for clamping the plate, assuming just 0.108" of plate being clamped, and brass blocks 1/4" thick. So far the force has dropped to 3.0 lbf...
rpm63: how exactly is the plate clamped?? Also, can you tell us the geometry and forces for the simply supported test you did?? That might eliminate some uncertainty to do with clamping.
I'm not familiar with a "pull tester." Is there a machine ID so we can look at an example on the Instron website??
Finally, I agree with dpadler1 about a sanity check with a couple of weights and a rule or dial gauge. What was the other machine (the "completely different" one) you checked??
Sorry to lump in so many queries at once.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
What I meant is this :
If you apply a point load to a plate at the center of the overhung edge, the edges of the plate do not deflect as much as the center. The wider the plate is, the greater the effect will be. If it is very wide (say with a 100:1 aspect ratio), the majority of the plate will deflect hardly at all and all the deformation will be in a small region close to the load. The simple beam calculation assumes a line load evenly distributed along the edge, so from the principle of virtual work, it follows that the deflection predicted by a hand calculation should be exceeded at the point of application of the load by both the true deflection and the FEA prediction. Now it is possible that this may not remain true for a plate of about 1:1 aspect ratio, so I might have to take my statement back, although intuitively it would seem to me that it would still be true. I wish I had access to an FEA program (which at this moment I don't).
RE: FEA Model versus Actual Results
From what you have described here, it sounds like a discrepancy between your testing methods and your FEA. dpadler sounds like he is on the right track with the instrument tolerances. Typical rule in testing is that you should be operating within 20-80% of the load cell range to get the specified accuracy of the load cell. Therefore, you should have at most a 10# load cell on your Instron, or at least have the gain set to limit the output range of the load aquisition equipment, with the first option being prefereable.
Check your load cell accuracy and capability, and the gain level of the acquisition equipment, then determine if this produces acceptable tolerances. If the load cell were to be above 100# capacity... I'd strongly recommend doing a basic high school test in which a known weight is added to the end of the beam and deflections measured using a dial gauge. It is too easy to get caught up in technology and loose sight of the limitations which it carries.
Sometimes simpler is better. Hope this helps.
jetmaker
RE: FEA Model versus Actual Results
The accuracy of the load cell was in the 20-80% scale range. I also did an accuracy/sanity check with dead weights and it checked out.
Unfortunately do not have the capability to find E with my pull tester other than an indirect method of working backward with a hand calculation for a cantilever. I would have to go out of house for testing and budgets are very tight. Multiple people mentioned previously that published E values should be close. However, I have not totally ruled out this possibility.
Thanks Rpstress for checking my FEA model with your model. I figured it would be good because is very close to hand calculations.
The part was clamped between two blocks.
The completely different method of testing is the following. I strapped a hand held digital force gage to a CNC mill with a manual z-axis. Even though it was a very crude set up, it was not far off from the Instron data. This appears to verify the equipment accuracy. I will also try a dial force gage.
The Instron model is 5544.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
Alternately, fix your physical test without bolting anything down, such that it is consistent with only translational constraints and no rotational constraints. Compare this physical test with the equivalent numerical/FEA results. If these are closer in agreement, then this definitely suggests that there is a divergence in the fixturing assumptions vs. the physical fixture.
This is a tough nut to crack.
Brad
RE: FEA Model versus Actual Results
At this point these seem the likely suspects:
Interpretation of force vs. deflection - I've seen people read force and deflection straight off the test results, without subtracting out the take-up compliance. You have to project down the linear part of the curve to establish zero deflection. This is important with manual checks as well, you have to get 3 points to make sure you are really in a linear range and project zero, subract that from your deflections. "Zeroing" the equipment does not mean you don't have to do this.
Yield during clamping on cantilever test- if the clamping force is enough to yield the sample you'll get higher deflections when loaded.
Warping during simply supported test - if you used the same size sample you can only get about 0.010" deflection before yield (assuming 50 ksi yield); could easily have .005" warpage in this size sample. Not a problem - if you project zero deflection as above. Effect is reduced with a longer thinner sample, and deflections higher so easier to measure accurately.
Yielding during testing - copper doesn't have a sharp yield point; depending on whether they gave you the right material and your sample size you could be getting into yield, which goes back to ensuring linearity.
The fact steel is also lower than predicted indicates some sort of testing issue or combination of issues. Unless there's something we're all missing about bending of work hardened materials not behaving as linear elastic. 50% is just too far off.
RE: FEA Model versus Actual Results
I did subtract out take up compliance. The measured curves are always linear.
I believe my original simply supported fixturing had some problems. I chose a thick piece of steel and consequently had high forces with very small deflections. I may have had some inaccuracies due to slippage in the fixturing. The difference between measured (Instron) vs. FEA for 2 different simply supported materials ranged from 8-17%. An improvement from the
I changed my clamping method to a vise that has a much higher clamping force. This appeared to help. Cantilever results Instron vs. FEA went from 30% to 19% difference. FEA force is always higher.
8-19% difference between FEA and measured results is much closer than 20 – 50% I originally reported.
RE: FEA Model versus Actual Results
Applying the enforced deformation right on one corner of the brass plate gives 2.53 lb as opposed to 3.0 lb, but applying it 10% of the plate's width to one side gave only 2.98 lb. This is with a crude representation of the clamping blocks, which is probably still a little over-stiff. Non-linear analysis gives 12% higher forces than linear analysis...
Re plate deformed shape, the FE predicts deflection at the free corners of the brass plate of 0.387", as opposed to 0.04" at the applied enforced deformation in the exact center, for both linear and non-linear results.
Is it possible to report/generate a simply supported beam result, to (largely) eliminate questions about the degree of fixity for the cantilevered plates?
RE: FEA Model versus Actual Results
Please elaborate/rephrase on the following:
Re plate deformed shape, the FE predicts deflection at the free corners of the brass plate of 0.387", as opposed to 0.04" at the applied enforced deformation in the exact center, for both linear and non-linear results.
Is it possible to report/generate a simply supported beam result, to (largely) eliminate questions about the degree of fixity for the cantilevered plates?
RE: FEA Model versus Actual Results
However, the deflection across the free end of the plate isn't varying much according to my analysis: the center of the end of the plate, where I'm applying a point-enforced deflection, is moving 0.04", just as I told it to. The corners of the free end of the plate are moving almost as much (0.0387"), so that this being a plate rather than a beam is not affecting the deflected shape too much. This is not directly relevant to your problem!
#2: on Jul 22, 2003 you posted that "...so I created a simply supported test along with a FEA model". I was thinking that maybe you could reprise the test and/or tell us more about it. For instance, analysing the little brass plate that I've been doing as a cantilever as a simply supported plate, I get a force of 51.7 lb for 0.04" deflection. I also get high stresses! It's a bit short and wide to analyse as a beam like this without some corrections, though the FE model should still be behaving more or less like reality. Also, how you're applying the deflection in terms of the shape and radius (?) of whatever is pressing on the plate may make a difference here.
Can you tell us more about your simply supported test??
RE: FEA Model versus Actual Results
Test Setup:
C260 Brass, 115mm long x 19 wide x .83 thick. Specimen was supported on two steel dowel pins and a point load applied in middle.
Measured results: deflection = 1mm, F=2.7N, deflection=3mm, F=8.1N
FEA:
2D, 4 elements though thickness, BC left end constrained x, y and z. Right end constrained z. Deflection=1mm applied at center. E=110320N/mm, (16,000,000 psi)
FEA results: deflection=1mm, F=3.15N. deflection=3mm, F=9.45N,
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
I've been having trouble finding good data on E for brass. The one wrought brass I've got a good value for is C240 to British aerospace spec B11. This gives an E of 100 GPa (14.5 Msi). MIL-HDBK-5J lists cast Al bronzes (a sort of brass) and gives low moduli (15 or 14.2 Msi, 103 or 98 GPa).
All other sources I've looked at on the web tend to give a blanket value of 110 GPa/16 Msi, for both C240 and C260.
I *suspect* that the E of 16 Msi is 10% high. I'd like some more authoratative data, though.
If 100 GPa is nearer the mark than 110 then it makes analysis/test = 2.88/2.7 = 1.067. 6-2/3% is still a bit high, in my opinion. The actual test specimen, being on round dowels, may see some effective shortening as it deflects and "rolls" around the dowels a little bit. Along with the reactions from the dowels then being slightly angled inwards, I'm not too sure of the detailed effects. However, the good linearity of the test data for 1.0 and 3.0 mm (8.1 N / 2.7 N = 3.0) indicates that this isn't a significant effect in this case.
Can anyone help with a better modulus? I'm not too familiar with copper alloys. We tend to use them only for bushes, and not very often at that.
RE: FEA Model versus Actual Results
Cheers
Greg Locock
RE: FEA Model versus Actual Results
Another problem could be other deformations in your test assembly.
RE: FEA Model versus Actual Results
My question is, where exactly is your force applied?- at the corner or in the middle. As English Muffin pointed out, transverse deformation does play a role.
I set up an FEA model with the info that RPM63 gave. I actually got about 3.25 lbs.
Once I changed the location to the corner and 'adjusted' the E by 10% (used 14.3 million psi instead of 16 million), I got exactly 2.4 lbs.
This is assuming that the clamps really worked and held it like a weld.
RE: FEA Model versus Actual Results
The low end here would give an error of 2.94/2.88 = 8.9%. Using the average (which I suppose you'd have to do in the sort of check usage rpm63 wants) gives 11.1%. Depending on your specimen this could amount to an error between 8% and 14%...too much for my taste.
Can live with this, rpm63? If not, perhaps a periodic check could be made on modulus. Anyone know how much a tensile modulus test would cost (probably something like five specimens, initially)?? bear in mind rpm63 has a tight budget...
In the next couple of weeks I hope to do some more detailed FE checking of the simply supported setup, with the dowels, etc., modeled.
I'm not sure how else to proceed here. Anyone??
RE: FEA Model versus Actual Results
Contact your local college/university. They may be willing to do the tests for you as part of one of their class experiments. It might cost you a few bucks, or some material as a donation to the department. It would be worth a try.
RE: FEA Model versus Actual Results
it would be a good time for rpm63 to summarize his progress and what new steps he has taken in resolving the discrepancies.
thus far the following issues have been identified in the dialog (17 pages worth, so I have glossed over some of them):
1. improper clamping (the modulus of the jaws must be greater than the material being tested for example)
2. recognition that while the Euler beam model(hand calc) appears to match the experimental result while in reality 2-d plate deflections are occurring; thus the agreement is somewhat fortuitous
3. the modulus of the beam material as well as precise unit conversions appear to be as yet un-resolved
4. dimensional tolerences of the test beams needs to be better defined as well as the specifics of how the beam is clamped.
RE: FEA Model versus Actual Results
Hacksaw:
1) yes, jaws made of steel.
2) Hand calcs don’t match experimental values. Hand calcs match FEA. I assume you meant to say this.
3) Unit conversions are not an issue.
4) Dimensional tolerance is negligible and was checked with measurements.
RE: FEA Model versus Actual Results
Any updates on this rpm63?
I am fairly new to this forum. 52 postings !!! Am I to assume all that discussion finally amounts to nothing.
wish there was a conclusion to this.
RE: FEA Model versus Actual Results
A lot of invaluable info in this thread. I can't resist adding a comment from my previous experience in benchmark: The theorical clamp or support are always very difficult to match with the real bench. So, can you measure 2 or 3 points along the "beam" and compare with the theorical profile ? (use the FEA plot and compare)
Why: If the theorical force is higher than the bench for the same deflection, it is likely to come from small rotations or displacements of your bench. It happens for your clamp and also your simply support tests. More difference with the clamp because the 0 rotation is quite impossible. By the way, that's the reason why people used to get the modulus from a 3 point bending (May be they do it now by resonance ?) Also, I have no doubt that the FEA matches with the hand calcs because these 2 methods use the same math formulas (for beam at least) and same 0 rotation, 0 displacement assumptions. Eventually, if you could model in FEA the beam and some jaws, that would make it.
RE: FEA Model versus Actual Results
good comments, however it is still unclear from the original posting if the original calculation was actually based on Euler beam elements or not.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results
rpm,
you need to bench mark your FEA code. there are a number of papers that deal with the weaknesses of some of the commercial codes.
typically you have to start with the beam cases for which exact analytical models exist and compare your results with the published results. there are some papaers that deal with flat plates under various b.c. that are compared with experimental testing.
you'll find that all FEA codes are not the same.
as part of the forum interaction you can propose a circular or rectangular beam with specified properties (don't model actual mat. properties yet) and tab. results for various b.b. and aspect ratios. that will help focus on where the problem lies.
good luck
RE: FEA Model versus Actual Results
please reread this thread; this is not an issue of the FEA code being in error, as the FEA results agree with theory. Rather, this is an issue of the FEA and theory not agreeing with experiment.
Brad
RE: FEA Model versus Actual Results
when the FEA model agrees with the simplified Euler-Bernoulli theory without shear or rotation, especially in the case of a flate plate(!) that introduces additional dimensionality, one is naturally interested in bench marking the FEA model, if for no other reason than to demonstrate its validity.
ours took about six-weeks.
RE: FEA Model versus Actual Results
RE: FEA Model versus Actual Results