Guide to Material Calibration –
Updated: Feb 8, 2021
Why, When and How Medical Device Designers and Analysts Should Perform Material Calibration
By Hicham Farid, PhD CAE/FEA Engineer at Aventec
The understanding of material behavior is the most important key for a successful realistic numerical simulation. Standard engineering materials behavior are well documented as many codes and standards are dedicated to provide either the material models or specify procedures on how to obtain proper material models. This is generally true for most common engineering materials such as composites, metals, and polymers.
With the considerable advances in medical devices, either from technology or manufacturing perspectives, the challenge worth overcoming is knowing the material behavior in order to perform high fidelity simulation. Either when talking about biological materials such as bone, skin, muscle tissue, or blood, or when talking about implants such as cervical cages, hip implants, coronary dilatation catheters, or stents. The first challenge that arises is; do we know our material and its behavior or not?
In this paper, I will be discussing different methodologies to calibrate material models versus test data for medical materials including metals, composites, and bio tissues. I will be using Abaqus and Isight to calibrate some example material models against test data while challenging the nonlinear nature of most of these materials. In the end, I will be able to answer the question we started with: Why and When should an analyst perform material calibration as part of a design and analysis workflow.
Figure 1. Experimental Data versus 3rd order Ogden Hyperelastic Material Model for Rubber
Metals, Rubbers and Bio-Tissue
When simulating a simple metallic component’s behavior under a simple static load, the engineer intuitively choses the Young’s modulus and the Poisson’s ratio adequately from a relevant book as most metals material parameters are well documented in handbooks and standards, etc. Still within metals, this assumption fades away as soon as we are investigating more complex behavior trends, such as plasticity, creep, fatigue, where classic elasticity theory does not apply anymore.
Industrial rubbers are another challenging material to work with. Their behavior is highly nonlinear even when they are exhibiting some sort of elasticity. Rubbers usually can be stretched further than 200% strains while staying elastic, this behavior is known as hyperelasticity. This class of material models requires the use of a strain energy potential to model adequately the material behavior.
Bio-tissues such as muscle, arterial walls, heart tissue, etc. are highly nonlinear materials. They often challenge the classical models at many levels as they present high level of hyperelasticity, rate dependency, and anisotropy. When these materials are subjected to small deformations (less than 2–5%), their mechanical behavior can generally be modeled adequately using conventional anisotropic linear elasticity. Under large deformations, however, these materials exhibit highly anisotropic and nonlinear elastic behavior due to rearrangements in the microstructure, such as reorientation of the fiber directions with deformation. The simulation of these nonlinear large-strain effects calls for more advanced constitutive models formulated within the framework of anisotropic hyperelasticity.
The Easy Way: Using Abaqus
For metals, describing the post yielding behavior relies most of the time on work hardening models. Abaqus/CAE allows to calibrate a material model from test data. With this capability, material test data can be imported into Abaqus/CAE, process the data, and derive elastic and plastic isotropic material behaviors from the data.
Figure 2. Stress-Strain experimental data of an Aluminum Alloy as imported to Abaqus/CAE
Once a calibration task is created, raw experimental data can be imported directly to CAE, then a curve fitting is performed in order to determine the elastic-plastic data of the material. Young’s modulus, Poisson’s Ratio, and the hardening curves are subsequently evaluated.
The calculated data can therefore be exported into the material definition module within Abaqus/CAE for subsequent use in the model preprocessing task.
Figure 3. Edit Behavior window
Figure 4. Stress-Strain data: Experimental versus Evaluated
Unless we are dealing with damage investigation, or with forming simulation (deep drawing, stamping, clod forming, etc.), we rarely use plasticity data as part of material definition for metals, as a simple elastic linear isotropic model could reproduce the expected behavior. Plugging the Young’s modulus and Poisson’s ratio directly into the material module box, or using the calibration tool as shown above, it is a straightforward approach either way.
When dealing with rubber-like materials, a high degree of elastic nonlinearity is always expected. Abaqus/CAE has a straightforward way to evaluate many hyperelastic material models using experimental data imported directly as part of the material definition.
Figure 5. Different Hyperelastic Material Models Available within Abaqus/CAE
Here, I used experimental stress-strain data of a conventional rubber material. I imported the raw Nominal (Engineering) stress-strain data into the material module. A simple right click on the material name from the model tree in CAE show the Evaluate sub-menu.
Different classes of hyperelastic models are available within the Evaluate Material menu. I usually picked the most common models to see which one fits my data the most.
Figure 6. Experimental Data different Hyperelastic Material Models
From Figure 6 we can conclude that Arruda-Boyce and Van Der Vaals models fit the experimental data the best. This is a simple illustration of Abaqus/CAE capability to evaluate hyperelastic material models data. Although, when a rubber part is confined during a simulation, simple uniaxial tensile test data are not sufficient. It is highly recommended that the analyst should include different types of test data into the evaluation process, such as biaxial and shear data.
Despite the extensive list of hyperelastic material models available within Abaqus/CAE Evaluation Module, it is limited to isotropic material. The challenge raised is when we are dealing with highly hyperelastic materials that exhibit a high degree of anisotropy, such bio-tissues (muscles, arterial walls, heart tissue, etc.). A more dedicated class of mathematical models can be used for this purpose.
However the expression of those models are quite complicated and need more dedicated optimization tools to calibrate. In the next section below we are going to investigate how I used Isight along with Abaqus in order to calibrate the Holzapfel anisotropic hyperelastic model for arterial layers simulation.
The Fancy Way: Using Isight with Abaqus
Modeling soft biological tissue problems are quite challenging giving their highly material nonlinaerities, coupled also with their anisotropy. As mentioned above, these tissues required more sophisticated models that couple their hyperelasticity nature along with the anisotropy.
One of the widely used models in literature to model the mechanical response of the adventitial layer of human iliac arteries is Holzapfel. The model is already implemented within Abaqus/CAE, however calibrating this model is quite challenging.
In this section I will be going through the calibration process of the Holzapfel anisotropic hyperelastic model using Isight and Abaqus. In an Isight Sim-Flow, I combined the optimization process component with Data Matching application component along with Abaqus.
Figure 7. Isight-Abaqus calibration sim-flow
I setup a one element cube model within Abaqus with simple tension load and boundary conditions. Setting the Abaqus component within Isight was straight forward, it does read the .cae file and import all the required data. It does defined the input as the material parameters and the outputs as the forces and displacement vectors.
After I setup the Data Matching component where I imported the experimental data as target and define the different parameters. Setup the optimization component in order to drive the calibration process. I used Hook-Jeeves algorithm with 250 iterations.
Figure 8. Experimental Data versus First Guess Data
As it was out of reach to get real experimental data. The experimental data I used here were reproduced from another numerical simulation. Therefore the results I obtained were not very reliable, but the focus was more on the developed methodology rather than the quality of the results.
The Sophisticated Way: Using AI Based Methods – Neural Networks
The main idea behind material calibration is minimize the error between a mathematical model and a set of experimental data. In its essence, it is an optimization problem. Classically, optimization problems have been solved using classical algorithms such as Least Squares.
With emergence of new Artificial Neural Networks few decades ago, their use ranges from pattern recognition, signal processing, and optimization. In this paragraph, I will be referring to one of my previous publications about the use of Neural Networks to calibrate a hyperplastic material (Acrylonitrile butadiene styrene or ABS).
In this work, I used the multilayer perceptron as adopted neural network architecture. During a learning process, the neural network changes its behavior to allow it to move towards a clearly defined purpose. In other words, learning is adjusting the connection weights so that the outputs of the network are as close as possible to the desired outputs for all the used examples (examples are generally input vectors associated with output vector that are previously have an established behavior). My inputs here were the excitations vector (stresses in other words), while my outputs were the material model parameters.
Figure 9. Architecture of the used Neural Network: Multilayer Perceptron
In this example, I investigated two hyperelastic models; Ogden and Mooney-Rivlin. The network I used consists of an input layer, hidden layers and an output layer. The number of neurons in the output layer depends on the response contemplated by the network. For the first approximation identification program, two neurons are required in the output layer to give the response of the excitation. The two neurons outputs represent the materials parameters embedded in the Mooney-Rivlin and Ogden models, while the input of the network is the variance of the corresponding stresses. Whereas for the second or third approximation model, the output layer takes more than two neurons depending on the behavior model presentation.
Figure 10. Experimental Stress-Strain data versus Ogden and Mooney-Rivlin models
Although the obtained error using this approximation was acceptable (~10%), I ran another set of simulations using second order definition for both material models to compare the results. This helped reducing the modeling error to ~4%.
Figure 11. Experimental Stress-Strain data versus second order Ogden and Mooney-Rivlin models
In this paper we exposed different methodologies of material calibration. The choice of each method is a trade-off between the material nature and complexity, the fidelity of the numerical simulation and availability of experimental test data.
It is hard to speculate which method is more appropriate for medical devices or life science applications generally. But we can draw some simple lines to help the reader:
· Metals are generally modeled using Hook’s law using Young’s modulus and Poisson’s ratio in the elastic regime, plus a hardening or softening law depending on the application. In this case, Abaqus/CAE can cover most of the engineering applications with high accuracy.
· Rubbers are bit tricky to deal with even at a simple elastic deformation. Their behavior is generally modeled using hyperelasticity theory. Abaqus/CAE contains a large library of hyperelastic material models which covers most of the rubbers anticipated behavior.
· Bio-Tissues are quite complex from engineering point of view. They are highly anisotropic and hyperelastic. Which requires different class of material models. Coupling Abaqus with Isight unleashes another level of material calibration capabilities that helps overcoming more complicated material behaviors such as Bio-Tissues.
· Using Artificial Neural Networks is an artificial intelligence based algorithm material calibration process. The methodology was illustrated in the case of a polymer (ABS). The drawback of this methodology is the high need for experimental data for the learning process.
T. Christian Gasser, Ray W. Ogden and Gerhard A. Holzapfel, Hyperelastic modelling of arterial layers with distributed collagen fibre orientations, J. R. Soc. Interface (2006) 3, 15–35
A. I. Arroyave, R. G. Lima, P. A. L. S. Martins, N. Ramiao, R. M. N. Jorge, Methodology for Mechanical Characterization of Soft Biological Tissues: arteries, Procedia Engineering 110 ( 2015 ) 74 – 81.
H. Farid, F. Erchiqui, M. El Ghorba and H. Ezzaidi, Neural Networks Approach for Hyperelastic Behaviour Characterization of ABS under Uniaxial Solicitation, British Journal of Applied Science & Technology 4(32): 4480-4493, 2014, ISSN: 2231-0843