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?
Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!
FEA Model versus Actual Results 4
- Thread starter rpm63
- Start date
While 10 to 20% is less alarming than 30 to 50%, it's still rather a lot.
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?
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?
- Thread starter
- #42
RPstress:
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?
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?
#1: this goes back to a post by EnglishMuffin on Aug 6, 2003. It's about how these little plates don't quite bend the same as a beam, since they have a significant distribution of load across them as well as along them.
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??
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??
- Thread starter
- #44
Simply supported beam, tested 8/14.
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,
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,
If you go to it lists the modulus of brass as varying between 96 and 110 GPa. Using a value close to 96 gives you the right answer.
My shell model of the SS beam gives 3.18 N for 1.0 mm enforced deformation. With E = 100 GPa I get 2.88 N.
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.
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.
GregLocock
Automotive
You can back calculate the modulus by measuring the free-free vibration frequency of a uniform beam, if you know the density.
Cheers
Greg Locock
Cheers
Greg Locock
MToppenberg
Mechanical
The difference may lie in the direction of the forces acting on your model. The beam theory(finite element is a numerical calculation of the beam theory)assumes that during loading the direction of the forces on it stays the same (the direction regard to the neutral line stays the same). In practice this is not the case. There could be an ofset in the load direction. This induces other forces acting on it.
Another problem could be other deformations in your test assembly.
Another problem could be other deformations in your test assembly.
DonkeyDude
Mechanical
Load direction update is not an issue for such a small deflection.
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.
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.
I have some info on modulus from a query to AZoM.com . They got in touch with NAMTEC (National Metals Technology Centre), a UK outfit based in Swindon. These guys claimed a modulus between 102 and 108 GPa (14.8 - 15.7 Msi, or 15.2 Msi +- 2.9%). However, they didn't quote a source for those numbers. I'm getting back to them next week.
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??
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??
A suggestion on how to get the Young's modulus for the material in question.
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.
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.
Interesting dialog.
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.
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.
- Thread starter
- #53
Donkey Dude: The force applied is in the middle.
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.
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.
DonkeyDude
Mechanical
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.
Hi rpm63 and all,
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.
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.
- Thread starter
- #57
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
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.
- Status
Similar threads
