Hyperelastic Material Correlation 1

[wnmascare]

Hi everyone!

I'm going to perform a structural analysis of na offshore componente called bend stiffener. It is made of polyurethane and it undergoes large elastic deformation. In this case, I need to use a hyperelastic model. I have the simple tensile test data for the polyurethane.

In order to decide which Abaqus hyperelastic model I should use in the bend stiffener analysis, I tried to correlate each model with the tensile test data I have. I modeled the specimen by using its exactly dimensions, then, I fixed one end of the specimen and I applied the total displacement reported in the tensile test data, i.e., 74 mm, on the other end. Then, I used the card *NODE PRINT to saved the reaction force of that point on the .dat file. The displacement I applied was the displacement of the tensile tests machine moving head when the specimen broke. For the analysis, I used the following cards:

*HYPERELASTIC, TEST DATA INPUT, POISSON = 0.45, YEOH
*UNIAXIAL TEST DATA, SMOOTH = 3
0.0000, 0.000
4.3917, 0.020
7.1791, 0.048
9.2796, 0.072
10.6931, 0.096
11.6854, 0.120
12.4112, 0.148
12.9463, 0.168
.
.
.
49.1106, 2.924
49.4159, 2.936
49.7593, 2.948
50.0654, 2.960
**
*STEP, INC = 100, NLGEOM = YES
**
*STATIC
0.005, 1.0, 1E-15,
**
*BOUNDARY, OP = NEW, TYPE = DISPLACEMENT
CONST_NODE, ENCASTRE
FORCE_NODE, 1, 1, -74.0
**

I started by using Yeoh model, then I ran the same model for the other models (Mooney-Rivlin, Arruda-Boyce, Polynomial, etc.). Following, for each model, I plotted the force vc displacement diagram along with the experimental data and I have not found any correlation among the hyperelastic models and the experimental data by simulating the tensile test itself.

Is there any additional information I should input? Is it a good practice the model the specimen with its whole dimensions? Do you guys think this could the problem?

Thank you in advance.

 

[rstupplebeen]

Abaqus/CAE has a built in function to take test data and fit hyperelastic material properties to it by running 1 element simulations. I believe that this could be a good starting point for you. Once you down select to a few models you can take the model you have already developed and optimize the coefficients to minimize the disparity with the test data. My colleague will be presenting this method at the Simulia Customer Conference in May. After the presentation I believe the materials will be made available.

http://www.3ds.com/company/events/scc-2013/customer-papers/

"Reverse-engineering of Contact Lens Mechanical Properties from an In Situ Compression Test"

I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[wnmascare]

rstupplebeen, thank you very much for your reply.

I am not used to working with Abaqus/CAE for modeling purpose. I use to create the mesh and generate the .inp file by using Hypermesh, then I type the necessary Abaqus cards in the .inp file. I just use Abaqus/CAE for visualization of the results.

But, anyway... You mean that I should simulate this job by considering only one elemento, is that right?

Once again, thank you very much!

 

[rstupplebeen]

Abaqus/CAE has a built in routine to create an 'optimal' material model of each of it's hyperelastic models on a single element in perfect tension among other modes. I believe that this then could be used as a great starting point to choose an appropriate model and then use the detailed test model to refine your model further. I hope this helps.

Rob Stupplebeen

https://sites.google.com/site/robertkstupplebeen/

 

[wnmascare]

rstupplebeen, thank you very much again for your reply.

I got the results I expected. I just modeled the gauge section of the specimen, intead of modeling the whole specimen. Now, the results look much better and reliable.