Read time: 15 minutes
Target audience: CAE Analysts, Researchers
Material calibration involves determining the material parameters that accurately represent the behaviour of a material under various conditions. This process is crucial because the accuracy of simulations and the reliability of their predictions depend heavily on the material models used. Material calibration ensures that these models reflect the true physical properties, such as elasticity, plasticity, and viscoelasticity, of the material being analysed. In Abaqus, proper material calibration is needed to generate precise results for structural strength analysis, enabling engineers to predict how materials will respond to loads, deformations, and environmental conditions with high fidelity. This calibration often involves experimental data and iterative adjustments to achieve a good correlation between the simulation and real-world behaviour.
When simulating the behaviour of a simple metallic component under a static load, engineers often use the Young’s modulus and Poisson’s ratio from handbooks, as these properties are well-documented for most metals. However, this approach is not suitable for more complex behaviours like plasticity, creep, and fatigue, where classic elasticity theory does not apply.
Industrial rubbers are even more challenging. Their behaviour is highly nonlinear, even when showing elasticity. Rubbers can stretch over 200% and still remain elastic, a property known as hyper-elasticity. To accurately model this, a strain energy potential is needed.
Hyperelastic materials are described in terms of a “strain energy potential,” U(ε), which defines the strain energy stored in the material per unit of reference volume (volume in the initial configuration) as a function of the strain at that point in the material. The following forms of strain energy potentials available in Abaqus to model approximately incompressible isotropic elastomers:
The Process of Material Calibration in Abaqus
Let’s dig in deep with the help of an example material calibration of a hyper-elastic rubber.
Abaqus/CAE allows you to evaluate hyper-elastic material behaviour by automatically creating response curves using selected strain energy potentials. In addition, you can provide experimental test data for a material without specifying a particular strain energy potential and have Abaqus/CAE evaluate the material to determine the optimal strain energy potential. This data typically includes stress-strain curves obtained from material testing, such as tensile or compression tests.
Using Test Data
The properties of rubber-like materials can vary significantly between batches. Therefore, when using data from multiple experiments, all experiments should be conducted on specimens from the same batch of material, regardless of whether you or Abaqus compute the coefficients.
The uniaxial tension test is the most common and is typically performed by pulling a “dog-bone” specimen. The uniaxial compression test involves loading a compression button between lubricated surfaces.
The equibiaxial compression test is rarely conducted due to experimental setup challenges. Moreover, this deformation mode is equivalent to a uniaxial tension test, which is easier to perform. A more common test is the equibiaxial tension test, which creates a stress state with two equal tensile stresses and zero shear stress by stretching a square sheet in a biaxial testing machine.
Planar tests are usually conducted using a thin, short, and wide rectangular strip of material, fixed on its wide edges to rigid loading clamps that are pulled apart.
When data from multiple experimental tests are available, such as uniaxial and equibiaxial test data, the Ogden and Van der Waals models provide the most accurate fit for experimental results. If limited test data are available, the Arruda-Boyce, Van der Waals, Yeoh, or reduced polynomial models are recommended. For only uniaxial test data, the Marlow or Valanis-Landel models are preferred. If only equibiaxial or planar test data are available, the Marlow model is recommended, as it constructs a strain energy potential that reproduces the test data exactly and behaves reasonably in other deformation modes.
Once the test data is inputted, a material calibration task can be created to identify the best-fitting strain energy potential.
Calibrating Material Coefficients
Abaqus can calibrate the material coefficients of hyper-elastic models from experimental stress-strain data, except for the Hencky model. For the Marlow and Valanis-Landel models, the test data directly define the strain energy potential, as these models do not use material coefficients. You can specify the value of N and provide experimental stress-strain data for up to four simple tests: uniaxial, equibiaxial, planar, and, for compressible materials, a volumetric compression test. Abaqus will compute the material parameters using a least-squares-fit procedure, which minimizes the relative error in stress.
Different strain energy potentials have different forms of Strain Energy (U), with material parameters and strain invariants. The polynomial form of the strain energy potential is one that is commonly used. Its form is
Where, U is the strain energy potential; Jel is the elastic volume ratio; I1 and I2 are measures of the distortion in the material; and N, Cij, and Di are material parameters, which may be functions of temperature. The Cij parameters describe the shear behavior of the material, and the Di parameters introduce compressibility.
When defining a hyperelastic material using experimental data, you must also specify the strain energy potential to be applied. Abaqus utilizes the experimental data to compute the coefficients for the chosen strain energy potential. It is crucial to ensure that there is a good correlation between the predicted material behavior and the experimental data.
The Material → Evaluate option allows you to calculate the material response using the specified strain energy potential based on the experimental data. If you are unsure which strain energy potential to choose, you can select “Unknown” from the Strain Energy Potential list in the material editor. Then, you can use the Evaluate option to perform standard tests with the experimental data across multiple strain energy potentials.
Upon completion of the tests, Abaqus/CAE enters the Visualization module and displays X-Y plots of the test results. Each plot shows the experimental data and a curve for each evaluated strain energy potential. Additionally, Abaqus/CAE provides a dialog box with the stability limits and coefficients for each strain energy potential.
Model Prediction of Material Behaviour v/s Experimental Data
Once the strain energy potential is determined, the behavior of the hyper-elastic model in Abaqus is established. However, it is essential to evaluate the quality of this behavior by comparing the predicted material response under various deformation modes with experimental data. You need to determine if the strain energy potentials computed by Abaqus are acceptable based on their correlation with the experimental results. This assessment can be performed automatically in Abaqus/CAE, or by using single-element test cases to derive the nominal stress–nominal strain response of the material model.
Material Stability
Abaqus checks the stability of the material under six different loading conditions: uniaxial tension and compression, equibiaxial tension and compression, and planar tension and compression, for 0.1≤𝜆1≤10.0 (nominal strain range of −0.9≤𝜖1≤9.0) at intervals of Δ𝜆1=0.01. If an instability is detected, Abaqus issues a warning and reports the lowest absolute value of 𝜖1 where the instability occurs. Ideally, no instability should be found. If instabilities are observed at strain levels likely to occur in the analysis, it is strongly recommended to either change the material model or carefully review and adjust the material input data.
Practical Applications of Material Calibration