Inaccurate fit of Hyperfoam material model

[nonlinearRus]

Hi all,

I am trying to fit a 2nd order Ogden Hyperfoam material model to my experimental data. The material is compressed uni-axially. The model doesn't seem to be a 2nd order model, and looks more like a 1st order N-H model. Also the Mu1,Mu2 and Alpha1,Alpha2 values are the same. Can anybody tell me why this is happening?
I have found a model in the literature that can model the behaviour much better, and I am wondering will I have to implement this model with the User language or am I making a silly mistake in using the Ogden model?

Any help much appreciated.

N

 

[Elabbasi]

According to the legend of your graph the experimental data is the magenta curve and the Ogden model gives the black curve? Are you sure it's not the opposite since I have not seen Ogden parameters that result in such a stress-strain curve.

If you use a second order Ogden model make sure the Alpha values are different even if you have to override the "optimized" values generated by the FE program.

If the fit to experimental data is still bad you should consider a different hyperelastic model that is available in Ansys. If none fit well then, as you mentioned, find a good model and code it yourself or get a pre-coded material library.

Nagi Elabbasi
Veryst Engineering

 

[nonlinearRus]

The black curve is actually the exp data, I don't know why but ANSYS somehow titles it as the model and titles the model as the experimental data.

I've just tried using the same model, increasing and fixing the Mu1 value (which controls the initial rise in the curve's elastic region). The curve now fits much better. The constants are now:
mu1 6000
Al1 0.949133384088
mu2 4.84106065038
al2 16.0952892458
b1 18.1994454263
b2 -0.0897630064121

Is there some sort of glitch in the curve fitting tool? I think that maybe I will have to use an external program (MatLab) to optimize the constants.

Thanks,

N

 

[nonlinearRus]

Here is the new curve fit

 

[Elabbasi]

That's a much better curve fit! The curve fitting for nonlinear materials is not a trivial optimization problem and it usually helps if the user nudges the program in the right direction, as you just did. Matlab gives you more control over the optimization but you have to code the material model equations yourself, so I wouldn't recommend it for a one time job.

One more things to look out for. You should, if possible, check the stability of the material based on the constants you selected. Ansys probably has a tool for that but I'm not sure. By stability I mean that the material stress strain curve can look nice as your does in uniaxial tension but in say planar compression could be unstable (stress goes down with increasing strain at some point).

Nagi Elabbasi

http://www.veryst.com

 

[nonlinearRus]

A much better fit alright! But I'm sure it could be better if I could optimize the parameters. So I've been trying to use the lsqcurvefit tool in Matlab Optimization toolbox, with little success!

My data is actually for uniaxial compression of a foam sample. The data was input into the uniaxial data section, and neither comp or tension was specified. So I don't know why it is down as tensile data! I also have shear data which I tried to implement into the model to improve the stability of the model. I'm not to sure how to analyse this. The model (magenta) that seems the fit the data (pink) is titled 'Experimental data trans'. The hyperfoam order 2 shear model doesn't fit as well. What is this experimental data trans curve? I've tried changing the model parameters again manually but to no avail.

The foam application will apply compression and shear, this is why these tests were chosen.


How does one go about analysing a model

 

[Elabbasi]

If your uniaxial experimental data is for compression, then put a minus sign before all stress and strain values. Regarding shear, I don't know what this "data trans" curve means. You are doing the right thing though by performing several experiments and trying to get the best overall fit.

In addition to Matlab optimization you can try third party software. Our company offers a material calibration tool called MCalibration. You can find more info on it on our website. Other FEA codes also have their own material calibration tools just like Ansys. You can use one of them, if you have access to other FEA codes, to find the better material constants (and then use them with Ansys).

Nagi Elabbasi

http://www.veryst.com

 

[nonlinearRus]

I've now fitted the data to the negative values and the plot is still titled uni-axial tension.

I'm still trying to get the MatLab optimization working properly though, and if I can't get much success I will look further into MCalibration - as it looks like a very useful tool.

I have a license of Abaqus available to me, I have yet to familirize myself with the package but I will do in due course.

Thanks for your help, much appreciated!