Hi everyone, in this video we’ll discuss • What are hyperelastic material models?
• Where are they used? • and how to calibrate them by curve-fitting
them to data in Workbench.
Let’s go!
Hyperelastic materials are a class of materials that can undergo deformations as large as
40% and sustain zero to negligible plastic deformation.
Materials such as rubbers, elastomers, soft tissues and foams typically exhibit this behavior.
The materials in this class share some common traits such as
• They’re soft in nature compared to most metals
• Their stress vs strain response is nonlinear and monotonically increasing
• Their stress vs strain curve follows the same path during loading and unloading.
This implies that all the work done in deforming them is conserved and it is stored as internal
energy which is fully recovered up on unloading.
This attribute of such materials is used in
defining their constitutive model in terms of strain energy density, which is the amount
of internal energy stored in a unit volume of the material.
The strain energy density is a function of the strain in the material and the stresses
developed in it are calculated based on the mode of deformation, so the response can differ,
depending on how the material is deformed.
So, to summarize, because of the complex stress-strain
relationship of elastomeric materials, hyperelasticity is typically defined with an equation, called
a strain energy potential.
Our challenge is to determine those coefficients of the equation
in order to characterize our material property, and that’s where experimental data from
controlled experiments come into play.
Typically, we perform tests in three modes
of deformation and calibrate, or curve-fit, for our hyperelastic coefficients.
These three modes of deformation are 1. Uniaxial tension
2. Uniaxial compression or biaxial tension 3. and in shear.
In addition to these, we also perform confined compression tests to calculate its volumetric
response. Together, these four data sets comprise a full set of data required to accurately
calibrate hyperelastic materials. In case of materials that are either fully or nearly
incompressible one may ignore the volumetric data under the assumption that the material
is fully incompressible.
It's worth noting that in practice one may
calibrate the hyperelastic model using test data in only one of these three modes of deformations.
In such cases, the model response may be reliable in only that mode of deformation.
Therefore, while it's possible to calibrate these models using data from only one mode
of deformation, it is highly recommended to use data from multiple or all three modes
of deformation.
The calibration of material model involves
selecting the hyperelastic model and curve-fitting it to the available experimental data.
As a result, we get constants which are considered as material properties.
There are several hyperelastic material models available in Ansys Mechanical that a user can pick from
and perform curve-fitting inside Engineering Data.
When we perform curve-fitting, we’re calculating the cumulative mismatch between the experimental
data and model prediction and minimize this value for an optimal set of material constants.
This error function is called as least squares function and depending on the nature of the
model and the number of material constants, either a linear or a nonlinear regression
method is used to minimize it.
The minimized value of this error function
is called as residue and it can be used to compare the quality of fit between two different models.
Now let’s look at a demo of how to perform
this curve fitting in Workbench using Engineering Data.
Here is the data for an elastomer sample, the data set includes uniaxial tension, biaxial
tension and in shear. This includes data in three modes of deformation, we don’t have
any volumetric data so it is assumed that the material is fully incompressible.
Notice that the three responses have a point of inflection in their response. This generally
implies that the material response may be made of two or more terms.
We’ll see how the quality of fit improves as we use models with more terms.
As a first step let’s open Workbench and insert a new static structural module.
Go to Engineering Data, add a new material, and name it as Elastomer.
Next, right mouse click and include property on uniaxial test data, biaxial test data and
shear test data from the toolbox under Hyperelastic Experimental Data.
Make sure that the project units are set to the same units as data and then copy the data
to the respective objects.
Next, we pick a hyperelastic model from the
toolbox and perform curve fitting. For starters, let’s use neo-Hookean model which is considered
a simple hyperelastic model.
You’ll notice that the option to perform
curve-fitting appears, notice that one case use either a normalized error or an absolute error.
This is same as the error function that we
discussed earlier, the difference between the two is that in case of normalized error
norm each datum is given equal weight during optimization.
The choice of error norm depends
on the data at hand, so it’s always recommended to check the quality of fit for both the norms
and pick the best.
Let’s solve the curve fit using normalized
error first. Here’s the solution, we can see that it follows the data fairly well but does
not capture the shape of the curve very well. Let’s change the error norm to absolute
and see if that makes any difference.
There’s not much improvement in the quality of fit so let’s proceed to add more terms.
Since neo-Hookean model only has one term we’ll use Yeoh 2nd order model which has
quadratic term in addition to the neo-Hookean model.
Once again, solve for the curve fit using normalized error.
While there isn’t much
improvement in the uniaxial and shear responses, the biaxial response is dropping down with
strain which indicates that it’s unstable. Let’s see if using absolute error gives
us a better fit. We can see that the quality of the fit is better compared to the normalized
error norm but it still doesn’t properly capture the shape of the curve.
Let’s add another term by using Yeoh 3rd order model. Solving for normalized error,
it’s hard to see how well the response is captured due to the auto limits on the axes.
Let’s change the limits on Y-axis to 0 to 3 MPa so we can make a better comparison.
Right click on Y-aixs and select Edit Properties.
Uncheck the automatic range and set the min.
and max. limits to 0 and 3 MPa.
Now we can see the quality of fit, it seems
to be capturing the inflexion point.
Let’s change the norm to absolute error and see
if there’s an improvement.
This is clearly a much better fit compared
to the models so far. There is still some room for improvement and perhaps one could
use better nonlinear models for better results but for the sake of this demo, let’s stop
brushing the apple and eat it! Before we proceed further, it’s important
to see if the calculated values make physical sense.
One way of doing this sanity check
is to calculate the initial shear modulus. For Yeoh 3rd order model this is nothing but
the 2 times C10.
Notice that one term has negative coefficient, but the total initial
shear modulus comes to be around 1.4 MPa which looks reasonable.
So, right click on the model and copy the calculated values to Property.
This completes the calibration of material model and now let’s go ahead to Mechanical and
perform a simulation using this model.
In this demo we’ll simulate the uniaxial
tension of a unit cube. The cube is fixed in X, Y and Z directions on three faces and
the other three faces are left free to deform. By doing so, we’re creating a state of uniform
deformation in the cube.
Attach the geometry and open Mechanical.
Assign material Elastomer to the body under Geometry in the tree.
Now define a mesh body sizing on the cube and set the element size equal to the length
of the side.
By doing so, we’re creating what is called as single element model.
This is a popular technique used for testing the response of material models as all other
model complexities are stripped off.
Select the face perpendicular to the X axis
and define a displacement condition and set X=0.
Now repeat the same step to fix the neighboring faces in Y and Z directions.
Next, select the other face that is normal to Y axis and define a displacement load of 0.7m.
This completes defining the loads and boundary
conditions. Next go to analysis settings and set large deformation to ON.
Hyperelastic models are nonlinear in nature and therefore they use large deflection theory.
Next, set the time stepping to off and set the number of sub-steps to 10. A typical simulation
using hyperelastic material models may benefit from using auto time stepping but due to the
simplicity of model we may turn it off. This completes the model setup, go ahead and
solve the model.
Now that the solution is available go ahead
and drag and drop the displacement object that was used to define loading to Solution
to create a force reaction probe to displacement object.
Note that the area of cross section of the cube in undeformed configuration is 1 meter square.
and the ratio of reaction force to initial area of cross section is engineering stress
in the material.
Therefore, the numerical value reported by this force reaction probe
is equal to the engineering stress in the part in Pascals units.
Also, the ratio of displacement in Y to it’s length in Y which is 1 m is same as engineering strain
Therefore, the numerical values reported by
the force-displacement chart from this unit cube are equal to the engineering stress and
engineering strain developed in the material.
So let’s go ahead and create a force-displacement
chart to extract this data in a table.
Select force reaction object and the displacement
object from model tress and insert chart.
Set the X axis to maximum of displacement, Set
Time to Omit. What we have here are equal to the values of engineering stresses and strains.
Comparing them against the data we input earlier,
we can see that they correlate very well.
This concludes the demo, now let’s summarize
what we learnt in this video. • Curve-fitting is used for calibrating
hyperelastic models based on experimental data.
• We need only one mode of deformation to calibrate the model but its highly recommended
to have data from all modes of deformation for accuracy.
• Remember that curve-fitting is only returning the optimum values, and user must verify the
values to check if they make physical sense before proceeding using them in analysis.
• Single element models are very useful in testing the material model since we can
achieve uniform deformation.
I hope that you found this video informative,
please share the video, post your comments, and subscribe to this channel to stay updated.
Don’t forget to visit courses.ansys.com to discover more useful courses.