Material properties: hyperelastic model for the rubber
You have been given some experimental test data for the rubber
material used in the mount.
Three different sets of test data—a uniaxial test, a biaxial
test, and a planar (shear) test—are available.
Context:
The data (shown in
Figure 1
and tabulated in
Table 1,
Table 2,
and
Table 3)
are given in terms of nominal stress and corresponding nominal strain.
Note:
Volumetric test data are not required when the material is
incompressible (as is the case in this example).
Table 1. Uniaxial test data.
Stress (Pa)
Strain
0.054E6
0.0380
0.152E6
0.1338
0.254E6
0.2210
0.362E6
0.3450
0.459E6
0.4600
0.583E6
0.6242
0.656E6
0.8510
0.730E6
1.4268
Table 2. Biaxial test data.
Stress (Pa)
Strain
0.089E6
0.0200
0.255E6
0.1400
0.503E6
0.4200
0.958E6
1.4900
1.703E6
2.7500
2.413E6
3.4500
Table 3. Planar test data.
Stress (Pa)
Strain
0.055E6
0.0690
0.324E6
0.2828
0.758E6
1.3862
1.269E6
3.0345
1.779E6
4.0621
When you define a hyperelastic material using experimental data, you also
specify the strain energy potential that you want to apply to the data.
Abaqus
uses the experimental data to calculate the coefficients necessary for the
specified strain energy potential. However, it is important to verify that an
acceptable correlation exists between the behavior predicted by the material
definition and the experimental data.
You can use the material evaluation option available in
Abaqus/CAE
to simulate one or more standard tests with the experimental data using the
strain energy potential that you specify in the material definition.
To define and evaluate hyperelastic material behavior:
Create a hyperelastic material named
Rubber. In this example a first-order,
polynomial strain energy function is used to model the rubber material; thus,
select Polynomial from the Strain energy
potential list in the material editor. Enter the test data given
above using the Test Data menu items in the material
editor.
To visualize the experimental data, click mouse button 3 on the table
for any of the test data and select Create
X–Y Data from the menu that appears. You
can then plot the data in
the Visualization module.
Note:
In general, you may be unsure of which strain energy
potential to specify. In this case, you could select
Unknown from the Strain energy
potential list in the material editor. You could then use the
Evaluate option to guide your selection by performing
standard tests with the experimental data using multiple strain energy
potentials.
In the
Model Tree,
click mouse button 3 on Rubber underneath the
Materials container. Select Evaluate
from the menu that appears to perform the standard unit-element tests
(uniaxial, biaxial, and planar). Specify a minimum strain of
0 and a maximum strain of
1.75 for each test. Evaluate only the
first-order polynomial strain energy function. This form of the hyperelasticity
model is known as the Mooney-Rivlin material model.
When the evaluation is complete,
Abaqus/CAE
enters
the Visualization module.
A dialog box appears containing material parameter and stability information.
In addition, an X–Y plot that displays a nominal
stress–nominal strain curve for the material as well as a plot of the
experimental data appears for each test.
The computational and experimental results for the various types of tests
are compared in
Figure 2,
Figure 3,
and
Figure 4
(for clarity, some of the computational data points are not shown). The
Abaqus/Standard
and experimental results for the biaxial tension test match very well. The
computational and experimental results for the uniaxial tension and planar
tests match well at strains less than 100%. The hyperelastic material model
created from these material test data is probably not suitable for use in
general simulations where the strains may be larger than 100%. However, the
model will be adequate for this simulation if the principal strains remain
within the strain magnitudes where the data and the hyperelastic model fit
well. If you find that the results are beyond these magnitudes or if you are
asked to perform a different simulation, you will have to insist on getting
better material data. Otherwise, you will not be able to have much confidence
in your results.
The hyperelastic material parameters
In this simulation the material is assumed to be incompressible
(
= 0). To achieve this, no volumetric test data were provided. To simulate
compressible behavior, you must provide volumetric test data in addition to the
other test data.
The hyperelastic material coefficients—,
,
and —that
Abaqus
calculates from the material test data appear in the Material
Parameters and Stability Limit Information dialog box, shown in
Figure 5.
The material model is stable at all strains with these material test data and
this strain energy function.
However, if you specified that a second-order (N=2) polynomial strain energy function be used, you would see the
warnings shown in
Figure 6.
If you had only uniaxial test data for this problem, you would find that the
Mooney-Rivlin material model
Abaqus
creates would have unstable material behavior above certain strain magnitudes.