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?
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-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
-
1
- #2
It appears that you are using beam theory for the theoretical answer. Are you also using beam elements for the FEA answer?
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
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
-
1
- Thread starter
- #3
I am not sure I understand the beam theory question. I am not using beam elements. 2 and 3-D models, 2-8 elements thick all yield similar 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)
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)
rpm63:
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
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
- Thread starter
- #5
EnglishMuffin
Mechanical
This doesn't sound like an FEA issue. Your cantilever beam is of such proportions that you should get good correlation with standard beam theory. Without seeing the experimental set up its difficult to come up with anything obvious, but some thoughts occur (probably irrelevant but you never know ):
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).
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).
- Thread starter
- #8
8 node bricks for 3D, 4 node for 2 D. I don't think it is the elements because the FEA results agree perfectly with the hand calculated formula. Also, I used different elements, 2D vs. 3D, coarse and fine meshes, and the results don't change much.
- Thread starter
- #9
EnglishMuffin:
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.
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.
EnglishMuffin
Mechanical
Well, if you are using a point load, I would not expect the correlation with simple beam theory to be quite so good, because of the transverse deformation. However, you say its good, so we'll ignore that. I would not have expected anisotropy caused by rolling to cause much anisotropy of the E value - but could be wrong about that. You could try the same simply supported test with a piece of steel - its simple enough. If that comes out right - it just has to be the E value that's the culprit.
EnglishMuffin
Mechanical
Another thought : How exactly are you measuring the force? Could your instrumentation be off ?
After more information, my beam issue was a red herring--the point of that was if you were actually using beam elements.
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
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
- Thread starter
- #13
Thanks for the input. I have been checking the instrumentation and it is a calibrated, accurate Instron pull test machine. I will attempt to do more instrumentation verification studies.
Have either of you done a similar bending test and come up with accurate FEA results vs. actual measurements?
Have either of you done a similar bending test and come up with accurate FEA results vs. actual measurements?
EnglishMuffin
Mechanical
In my experience, if you make a good model, for something as simple as you have here, I would say you ought to be able to get within a few percent. I was once involved with a guy at NIST who made a very accurate FEA model of a length standard bar, and predicted the sag within a fraction of a percent.
rpm63:
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
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
rpm63,
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
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
-
1
- #18
GregLocock
Automotive
One other approach is to predict the natural frequencies of the beam, unconstrained.
This is easy to measure accurately, in practice. Once this is correlated then you can look at boundary conditions.
Cheers
Greg Locock
This is easy to measure accurately, in practice. Once this is correlated then you can look at boundary conditions.
Cheers
Greg Locock
utpalborah
Mechanical
I joined this group a few days back only and this is my first communication.
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
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
-
1
- #20
This appears deeply bizarre.
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.
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.
- Status
Similar threads
- Question
- Question