0
$\begingroup$

load disp curves comparison results between FEM and Experimental results

According to my results, I can have this curves. And somehow in this figure, it is not pretty much similar, What can I say if it is asked why I still want to use the FEM results? Or how can I validate the FEM results from this figure?

Any help? I really appreciate it Thank you very much in advance

$\endgroup$
4
  • $\begingroup$ The Youngs modules seems very different. $\endgroup$
    – fibonatic
    Jul 27, 2018 at 17:40
  • $\begingroup$ Guess your material is tougher than the values you put into your FEM algo. The "soft" breakover shown in FEM suggests further that the material is more brittle than you programmed into the simulation. $\endgroup$ Jul 27, 2018 at 17:55
  • $\begingroup$ The real world does not match the computer ? The real world must be wrong.\. $\endgroup$ Jul 28, 2018 at 16:16
  • $\begingroup$ The real curve looks like a pretty typical hot rolled steel , has a yield point. The grips did not grab or threads seat, until there was some initial load. $\endgroup$ Jul 28, 2018 at 16:21

3 Answers 3

2
$\begingroup$

The tail end of the curve is probably not a massive issue as that is well into the region which would normally be considered failure in any case and FE systems often don't really look at failure mode in detail.

Of more concern is the elastic region where the FEM results suggest it is a lot stiffer than it is in the experiment. The experimental curve also doesn't follow a straight line at the start of the experiment which suggest that there is some slack being taken up somewhere. This could either be an issue with the experimental apparatus or the sample itself.

Without knowing the details of the part its is hard to speculate in detail but it could be say that you have bolted joints with inadequate preload and they are slipping under the initial loading.

The difference in Youngs modulus implies a more fundamental issue with the FE model though, perhaps an incorrect value for E or invalid assumptions about things like joint stiffness.

A likely possibility is that you have some elements of the model whcih are constrained in too many degrees of freedom compared to the experiment eg you have a rigid joint where you should have a pinned joint.

$\endgroup$
3
$\begingroup$

These look like some sort of tensile test on a ductile material which is loaded until it breaks.

In the experiment, it looks like the test rig has some "slack" which gets taken up when the load reaches about 25 kN. There may be some flexibility in the test rig that makes the slope of the elastic deformation different from the theoretical model of a perfectly rigid test rig, or you might simply have a different values of Young's modulus from the test material.

Quite likely the load is applied to the test piece in a different way in the FE model and the test. For example the test may be applying a relatively concentrated load via a pin through a hole in the specimen (and there may be local plastic deformation around the hole, the pin may be bending slightly, etc, etc), but the FE model may by applying a uniform tension across all the cross section.

The elastic limit is slightly different between the test and FE model, but the difference of 10% is nothing to be worried about. The experiment is done in the real world, not in some idealized environment where everything is known to 16 decimal places! If you are going to design some "real life" structure based on these results, you would probably have "safety factors" much bigger than 10% in any case.

At large displacements, presumably the FE model has some effect (material properties again?) which makes the load curve slope downwards, after some value of strain is reached. The test does the same thing but to a smaller amount.

You don't say what FE software you used, but you might have only defined the material properties up to the strain that corresponds to the deflection of 35mm. Make sure that Young's modulus doesn't suddenly jump to zero for higher strains in your FE model, or something similar and unrealistic!

The test specimen then suddenly broke. There is probably nothing in the FE model to represent that explicitly.

The general agreement between test and model is very good here IMO. You just need to sort out a few details. Either correct the test data for the defects in the test rig, or make a more detailed FE model that includes the same defects.

$\endgroup$
1
$\begingroup$

Well, two categories of questions come to mind straight away:

1) what values were used for the FEM? Are they based on the actual material tested? What was the source of those values and the confidence level?

2) what accuracy were the primary results measured to? Change in length for example - how was it measured? A plastic ruler or a digital vernier with 3 digit resolution?

Once you establish an error for the primary values, then you can work out an error for the result...

$\endgroup$
6
  • $\begingroup$ We considered 5 different cases, each cases has different variation of parameters, there are 10 parameters we considered: Initial Thickness, Plate width, length, average thickness, minimum average thickness, minimum thickness, standard deviation, young modulus, yield strength, ultimate strength. However we found that the error percentage for tensile strengh comparison results is 4.8% $\endgroup$ Jul 27, 2018 at 16:47
  • $\begingroup$ so if you run the analysis with +/- 4.8% how does that change the results? $\endgroup$
    – Solar Mike
    Jul 27, 2018 at 16:56
  • $\begingroup$ No , I meant, we had two comparison results, the tensile strength results and the load-disp results, from the tensile strength results, it was found the error was 4.8% using regression , but for the load-disp figure I attached, somehow it looks like the results are equivalent, but somehow still not much similar, how can I come up with a reason that FEM results are validated from this figure? $\endgroup$ Jul 27, 2018 at 16:59
  • $\begingroup$ So, is the experiment curve an average of the 5 cases? Or was one case picked to provide the input values for the FEM? $\endgroup$
    – Solar Mike
    Jul 27, 2018 at 17:01
  • $\begingroup$ Ah I forgot to tell that, it is per one case, so I only show one sample only, each case has one curve $\endgroup$ Jul 27, 2018 at 17:03

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.