Hyperelastic Behavior of Rubberlike Materials

Compressibility

Most elastomers (solid, rubberlike materials) have very little compressibility compared to their shear flexibility. This behavior does not warrant special attention for plane stress, shell, membrane, beam, truss, or rebar elements, but the numerical solution can be quite sensitive to the degree of compressibility for three-dimensional solid, plane strain, and axisymmetric analysis elements. In cases where the material is highly confined (such as an O-ring used as a seal), the compressibility must be modeled correctly to obtain accurate results. In applications where the material is not highly confined, the degree of compressibility is typically not crucial; for example, it would be quite satisfactory in Abaqus/Standard to assume that the material is fully incompressible: the volume of the material cannot change except for thermal expansion.

Another class of rubberlike materials is elastomeric foam, which is elastic but very compressible. Elastomeric foams are discussed in Hyperelastic Behavior in Elastomeric Foams.

We can assess the relative compressibility of a material by the ratio of its initial bulk modulus, $K_{0}$ , to its initial shear modulus, $μ_{0}$ . This ratio can also be expressed in terms of Poisson's ratio, $ν$ , since

$ν = \frac{3 K_{0} / μ_{0} - 2}{6 K_{0} / μ_{0} + 2} .$

The table below provides some representative values.


$K_{0} / μ_{0}$	Poisson's ratio
10	0.452
20	0.475
50	0.490
100	0.495
1000	0.4995
10,000	0.49995

Compressibility in Abaqus/Standard

In Abaqus/Standard it is recommended that you use solid continuum hybrid elements for almost incompressible hyperelastic materials with initial Poisson's ratio greater than 0.495 (i.e., the ratio of $K_{0} / μ_{0}$ greater than 100) to avoid potential convergence problems. Otherwise, the analysis preprocessor will issue an error. Except for fully incompressible hyperelastic materials, you can use the “nonhybrid incompressible” diagnostics control to downgrade this error to a warning message.

In plane stress, shell, and membrane elements the material is free to deform in the thickness direction. Similarly, in one-dimensional elements (such as beams, trusses, and rebars) the material is free to deform in the lateral directions. In these cases special treatment of the volumetric behavior is not necessary; the use of regular stress/displacement elements is satisfactory.

Input File Usage

Use the following option to downgrade an error message to a warning message:

DIAGNOSTICS, NONHYBRID INCOMPRESSIBLE=WARNING

Compressibility in Abaqus/Explicit

Except for plane stress and uniaxial cases, it is not possible to assume that the material is fully incompressible in Abaqus/Explicit because the program has no mechanism for imposing such a constraint at each material calculation point. Instead, we must provide some compressibility. The difficulty is that, in many cases, the actual material behavior provides too little compressibility for the algorithms to work efficiently. Thus, except for plane stress and uniaxial cases, you must provide enough compressibility for the code to work, knowing that this makes the bulk behavior of the model softer than that of the actual material. Some judgment is, therefore, required to decide whether or not the solution is sufficiently accurate, or whether the problem can be modeled at all with Abaqus/Explicit because of this numerical limitation.

If no value is given for the material compressibility in the hyperelastic model, by default Abaqus/Explicit assumes $K_{0} / μ_{0} = $ 20, corresponding to Poisson's ratio of 0.475. Since typical unfilled elastomers have $K_{0} / μ_{0}$ ratios in the range of 1,000 to 10,000 ( $ν = $ 0.4995 to $ν = $ 0.49995) and filled elastomers have $K_{0} / μ_{0}$ ratios in the range of 50 to 200 ( $ν = $ 0.490 to $ν = $ 0.497), this default provides much more compressibility than is available in most elastomers. However, if the elastomer is relatively unconfined, this softer modeling of the material's bulk behavior usually provides quite accurate results. Unfortunately, in cases where the material is highly confined—such as when it is in contact with stiff, metal parts and has a very small amount of free surface, especially when the loading is highly compressive—it may not be feasible to obtain accurate results with Abaqus/Explicit.

If you are defining the compressibility rather than accepting the default value, an upper limit of 100 is suggested for the ratio of $K_{0} / μ_{0}$ . Larger ratios introduce high frequency noise into the dynamic solution and require the use of excessively small time increments.

Isotropy Assumption

In Abaqus all hyperelastic models are based on the assumption of isotropic behavior throughout the deformation history. Hence, the strain energy potential can be formulated as a function of the strain invariants.

Strain Energy Potentials

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. There are several forms of strain energy potentials available in Abaqus to model approximately incompressible isotropic elastomers: the Arruda-Boyce form, the Marlow form, the Mooney-Rivlin form, the neo-Hookean form, the Ogden form, the polynomial form, the reduced polynomial form, the Yeoh form, the Valanis-Landel form, and the Van der Waals form. As will be pointed out below, the reduced polynomial and Mooney-Rivlin models can be viewed as particular cases of the polynomial model; the Yeoh and neo-Hookean potentials, in turn, can be viewed as special cases of the reduced polynomial model. Thus, we will occasionally refer collectively to these models as “polynomial models.”

Generally, when data from multiple experimental tests are available (typically, this requires at least uniaxial and equibiaxial test data), the Ogden and Van der Waals forms are more accurate in fitting experimental results. If limited test data are available for calibration, the Arruda-Boyce, Van der Waals, Yeoh, or reduced polynomial forms provide reasonable behavior. When only uniaxial test data is available, the Marlow or the Valanis-Landel form is recommended, and the Marlow form is recommended if only equibiaxial or planar test data is available. In this case, a strain energy potential is constructed that reproduces the test data exactly and that has reasonable behavior in other deformation modes.

Evaluating Hyperelastic Materials

Abaqus/CAE allows you to evaluate hyperelastic material behavior 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. See Evaluating hyperelastic, hyperfoam and viscoelastic material behavior for details. Alternatively, you can use single-element test cases to evaluate the strain energy potential.

Arruda-Boyce Form

The form of the Arruda-Boyce strain energy potential is

$\begin{matrix} U = & μ {\frac{1}{2} ({\bar{I}}_{1} - 3) + \frac{1}{20 λ_{m}^{2}} ({\bar{I}}_{1}^{2} - 9) + \frac{11}{1050 λ_{m}^{4}} ({\bar{I}}_{1}^{3} - 27) \\ + \frac{19}{7000 λ_{m}^{6}} ({\bar{I}}_{1}^{4} - 81) + \frac{519}{673750 λ_{m}^{8}} ({\bar{I}}_{1}^{5} - 243)} + \frac{1}{D} (\frac{J_{e ℓ}^{2} - 1}{2} - \ln J_{e ℓ}), \end{matrix}$

where U is the strain energy per unit of reference volume; $μ$ , $λ_{m}$ , and D are temperature-dependent material parameters; ${\bar{I}}_{1}$ is the first deviatoric strain invariant defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2},$

where the deviatoric stretches ${\bar{λ}}_{i} = J^{- \frac{1}{3}} λ_{i}$ , J is the total volume ratio, $J^{e ℓ}$ is the elastic volume ratio as defined below in Thermal Expansion, and $λ_{i}$ are the principal stretches. The initial shear modulus, $μ_{0}$ , is related to $μ$ with the expression

$μ_{0} = μ (1 + \frac{3}{5 λ_{m}^{2}} + \frac{99}{175 λ_{m}^{4}} + \frac{513}{875 λ_{m}^{6}} + \frac{42039}{67375 λ_{m}^{8}}) .$

A typical value of $λ_{m}$ is 7, for which $μ_{0} = 1.0125 μ$ . Both the initial shear modulus, $μ_{0}$ , and the parameter $μ$ are printed in the data (.dat) file if you request a printout of the model data from the analysis input file processor. The initial bulk modulus is related to D with the expression

$K_{0} = \frac{2}{D} .$

Marlow Form

The form of the Marlow strain energy potential is

$U = U_{d e v} ({\bar{I}}_{1}) + U_{v o l} (J_{e ℓ}),$

where U is the strain energy per unit of reference volume, with $U_{d e v}$ as its deviatoric part and $U_{v o l}$ as its volumetric part; ${\bar{I}}_{1}$ is the first deviatoric strain invariant defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2},$

where the deviatoric stretches ${\bar{λ}}_{i} = J^{- \frac{1}{3}} λ_{i}$ , J is the total volume ratio, $J_{e ℓ}$ is the elastic volume ratio as defined below in Thermal Expansion, and $λ_{i}$ are the principal stretches. The deviatoric part of the potential is defined by providing either uniaxial, equibiaxial, or planar test data; while the volumetric part is defined by providing the volumetric test data, defining the Poisson's ratio, or specifying the lateral strains together with the uniaxial, equibiaxial, or planar test data.

Mooney-Rivlin Form

The form of the Mooney-Rivlin strain energy potential is

$U = C_{10} ({\bar{I}}_{1} - 3) + C_{01} ({\bar{I}}_{2} - 3) + \frac{1}{D_{1}} {(J^{e ℓ} - 1)}^{2},$

where U is the strain energy per unit of reference volume; $C_{10}$ , $C_{01}$ , and $D_{1}$ are temperature-dependent material parameters; ${\bar{I}}_{1}$ and ${\bar{I}}_{2}$ are the first and second deviatoric strain invariants defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2} and {\bar{I}}_{2} = {\bar{λ}}_{1}^{(- 2)} + {\bar{λ}}_{2}^{(- 2)} + {\bar{λ}}_{3}^{(- 2)},$

$μ_{0} = 2 (C_{10} + C_{01}), K_{0} = \frac{2}{D_{1}} .$

Neo-Hookean Form

The form of the neo-Hookean strain energy potential is

$U = C_{10} ({\bar{I}}_{1} - 3) + \frac{1}{D_{1}} {(J^{e ℓ} - 1)}^{2},$

where U is the strain energy per unit of reference volume; $C_{10}$ and $D_{1}$ are temperature-dependent material parameters; ${\bar{I}}_{1}$ is the first deviatoric strain invariant defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2},$

$μ_{0} = 2 C_{10}, K_{0} = \frac{2}{D_{1}} .$

Ogden Form

The form of the Ogden strain energy potential is

$U = \underset{i = 1}{\sum^{N}} \frac{2 μ_{i}}{α_{i}^{2}} ({\bar{λ}}_{1}^{α_{i}} + {\bar{λ}}_{2}^{α_{i}} + {\bar{λ}}_{3}^{α_{i}} - 3) + \overset{N}{\sum_{i = 1}} \frac{1}{D_{i}} {(J^{e ℓ} - 1)}^{2 i},$

where ${\bar{λ}}_{i}$ are the deviatoric principal stretches ${\bar{λ}}_{i} = J^{- \frac{1}{3}} λ_{i}$ ; $λ_{i}$ are the principal stretches; N is a material parameter; and $μ_{i}$ , $α_{i}$ , and $D_{i}$ are temperature-dependent material parameters. The initial shear modulus and bulk modulus for the Ogden form are given by

$μ_{0} = \overset{N}{\sum_{i = 1}} μ_{i}, K_{0} = \frac{2}{D_{1}} .$

The particular material models described above—the Mooney-Rivlin and neo-Hookean forms—can also be obtained from the general Ogden strain energy potential for special choices of $μ_{i}$ and $α_{i}$ .

Polynomial Form

The form of the polynomial strain energy potential is

$U = \overset{N}{\sum_{i + j = 1}} C_{i j} {({\bar{I}}_{1} - 3)}^{i} {({\bar{I}}_{2} - 3)}^{j} + \overset{N}{\sum_{i = 1}} \frac{1}{D_{i}} {(J^{e ℓ} - 1)}^{2 i},$

where U is the strain energy per unit of reference volume; N is a material parameter; $C_{i j}$ and $D_{i}$ are temperature-dependent material parameters; ${\bar{I}}_{1}$ and ${\bar{I}}_{2}$ are the first and second deviatoric strain invariants defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2} and {\bar{I}}_{2} = {\bar{λ}}_{1}^{(- 2)} + {\bar{λ}}_{2}^{(- 2)} + {\bar{λ}}_{3}^{(- 2)},$

$μ_{0} = 2 (C_{10} + C_{01}), K_{0} = \frac{2}{D_{1}} .$

For cases where the nominal strains are small or only moderately large (< 100%), the first terms in the polynomial series usually provide a sufficiently accurate model. Some particular material models—the Mooney-Rivlin, neo-Hookean, and Yeoh forms—are obtained for special choices of $C_{i j}$ .

Reduced Polynomial Form

The form of the reduced polynomial strain energy potential is

$U = \overset{N}{\sum_{i = 1}} C_{i 0} {({\bar{I}}_{1} - 3)}^{i} + \overset{N}{\sum_{i = 1}} \frac{1}{D_{i}} {(J^{e ℓ} - 1)}^{2 i},$

where U is the strain energy per unit of reference volume; N is a material parameter; $C_{i 0}$ and $D_{i}$ are temperature-dependent material parameters; ${\bar{I}}_{1}$ is the first deviatoric strain invariant defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2},$

$μ_{0} = 2 C_{10}, K_{0} = \frac{2}{D_{1}} .$

Valanis-Landel Form

The form of the Valanis-Landel strain energy potential is

$U = U_{d e v} ({\bar{λ}}_{1}, {\bar{λ}}_{2}, {\bar{λ}}_{3}) + U_{v o l} (J_{e ℓ}),$

where U is the strain energy per unit of reference volume, with $U_{d e v}$ as its deviatoric part and $U_{v o l}$ as its volumetric part. For the Valanis-Landel model it is further assumed that the deviatoric part of the strain energy potential, $U_{d e v}$ , is expressed as three separable but identical functions of principal deviatoric stretches

$U_{d e v} = F ({\bar{λ}}_{1}) + F ({\bar{λ}}_{2}) + F ({\bar{λ}}_{3}),$

where the deviatoric stretches ${\bar{λ}}_{i} = J^{- \frac{1}{3}} λ_{i}$ , J is the total volume ratio, $J_{e ℓ}$ is the elastic volume ratio as defined below in Thermal Expansion, and $λ_{i}$ are the principal stretches. The deviatoric part of the potential is defined by providing uniaxial test data; while the volumetric part is defined either by providing volumetric test data, by providing the uniaxial test data with lateral strains specified, or by defining the Poisson's ratio.

Van Der Waals Form

The form of the Van der Waals strain energy potential is

$U = μ {- (λ_{m}^{2} - 3) [\ln (1 - η) + η] - \frac{2}{3} a {(\frac{\tilde{I} - 3}{2})}^{\frac{3}{2}}} + \frac{1}{D} (\frac{J_{e ℓ}^{2} - 1}{2} - \ln J_{e ℓ}),$

where

$\tilde{I} = (1 - β) {\bar{I}}_{1} + β {\bar{I}}_{2} and η = \sqrt{\frac{\tilde{I} - 3}{λ_{m}^{2} - 3}} .$

Here, U is the strain energy per unit of reference volume; $μ$ is the initial shear modulus; $λ_{m}$ is the locking stretch; a is the global interaction parameter; $β$ is an invariant mixture parameter; and D governs the compressibility. These parameters can be temperature-dependent. ${\bar{I}}_{1}$ and ${\bar{I}}_{2}$ are the first and second deviatoric strain invariants defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2} and {\bar{I}}_{2} = {\bar{λ}}_{1}^{(- 2)} + {\bar{λ}}_{2}^{(- 2)} + {\bar{λ}}_{3}^{(- 2)},$

$μ_{0} = μ, K_{0} = \frac{2}{D} .$

Yeoh Form

The form of the Yeoh strain energy potential is

$\begin{matrix} U = & C_{10} ({\bar{I}}_{1} - 3) + C_{20} {({\bar{I}}_{1} - 3)}^{2} + C_{30} {({\bar{I}}_{1} - 3)}^{3} \\ + \frac{1}{D_{1}} {(J^{e ℓ} - 1)}^{2} + \frac{1}{D_{2}} {(J^{e ℓ} - 1)}^{4} + \frac{1}{D_{3}} {(J^{e ℓ} - 1)}^{6}, \end{matrix}$

where U is the strain energy per unit of reference volume; $C_{i 0}$ and $D_{i}$ are temperature-dependent material parameters; ${\bar{I}}_{1}$ is the first deviatoric strain invariant defined as

${\bar{I}}_{1} = {\bar{λ}}_{1}^{2} + {\bar{λ}}_{2}^{2} + {\bar{λ}}_{3}^{2},$

$μ_{0} = 2 C_{10}, K_{0} = \frac{2}{D_{1}} .$

Thermal Expansion

Only isotropic thermal expansion is permitted with the hyperelastic material model.

The elastic volume ratio, $J^{e ℓ}$ , relates the total volume ratio, J, and the thermal volume ratio, $J^{t h}$ :

$J^{e ℓ} = \frac{J}{J^{t h}} .$

$J^{t h}$ is given by

$J^{t h} = {(1 + ε^{t h})}^{3},$

where $ε^{t h}$ is the linear thermal expansion strain that is obtained from the temperature and the isotropic thermal expansion coefficient (Thermal Expansion).

Defining the Hyperelastic Material Response

The mechanical response of a material is defined by choosing a strain energy potential to fit the particular material. The strain energy potential forms in Abaqus are written as separable functions of a deviatoric component and a volumetric component; i.e., $U = U_{d e v} ({\bar{I}}_{1}, {\bar{I}}_{2}) + U_{v o l} (J_{e ℓ})$ . Alternatively, in Abaqus/Standard you can define the strain energy potential with user subroutine UHYPER, in which case the strain energy potential need not be separable.

Generally for the hyperelastic material models available in Abaqus, you can either directly specify material coefficients or provide experimental test data and have Abaqus automatically determine appropriate values of the coefficients. An exception is the Marlow form: in this case, the deviatoric part of the strain energy potential must be defined with test data. The different methods for defining the strain energy potential are described in detail below.

The properties of rubberlike materials can vary significantly from one batch to another; therefore, if data are used from several experiments, all of the experiments should be performed on specimens taken from the same batch of material, regardless of whether you or Abaqus compute the coefficients.

Viscoelastic and Hysteretic Materials

The elastic response of viscoelastic materials (Time Domain Viscoelasticity and Parallel Rheological Framework) and hysteretic materials (Hysteresis in Elastomers) can be specified by defining either the instantaneous response or the long-term response of such materials.

Instantaneous Response

To define the instantaneous response, the experiments outlined in Experimental Tests have to be performed within time spans much shorter than the characteristic relaxation times of these materials.

Input File Usage

HYPERELASTIC, MODULI=INSTANTANEOUS

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; any Strain energy potential except Unknown: Moduli time scale (for viscoelasticity): Instantaneous

Long-Term Response

If the long-term elastic response is used, data from experiments have to be collected after time spans much longer than the characteristic relaxation times of these materials. Long-term elastic response is the default elastic material behavior.

Input File Usage

HYPERELASTIC, MODULI=LONG TERM

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; any Strain energy potential except Unknown: Moduli time scale (for viscoelasticity): Long-term

Accounting for Compressibility

Compressibility can be defined by specifying nonzero values for $D_{i}$ (except for the Marlow and Valanis-Landel models), by setting the Poisson's ratio to a value less than 0.5, or by providing test data that characterize the compressibility. The test data method is described later in this section. If you specify the Poisson's ratio for hyperelasticity other than the Marlow or the Valanis-Landel models, Abaqus computes the initial bulk modulus from the initial shear modulus

$D_{1} = \frac{2}{K_{0}} = \frac{3 (1 - 2 ν)}{μ_{0} (1 + ν)} .$

For the Marlow model and the Valanis-Landel model the specified Poisson's ratio represents a constant value, which determines the volumetric response throughout the deformation process. If $D_{1}$ is equal to zero, all of the $D_{i}$ must be equal to zero. In such a case the material is assumed to be fully incompressible in Abaqus/Standard, while Abaqus/Explicit assumes compressible behavior with $K_{0} / μ_{0} = 20$ (Poisson's ratio of 0.475).

Input File Usage

HYPERELASTIC, POISSON= $ν$

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: Material type: Isotropic; any Strain energy potential except Unknown or User-defined: Input source: Test data: Poisson's ratio:  $ν$

Specifying Material Coefficients Directly

The parameters of the hyperelastic strain energy potentials can be given directly as functions of temperature for all forms of the strain energy potential except the Marlow and Valanis-Landel forms.

Input File Usage

Use one of the following options:

HYPERELASTIC, ARRUDA-BOYCE
HYPERELASTIC, MOONEY-RIVLIN
HYPERELASTIC, NEO HOOKE
HYPERELASTIC, OGDEN, N=n ( $n \leq 6$ )
HYPERELASTIC, POLYNOMIAL, N=n ( $n \leq 6$ )
HYPERELASTIC, REDUCED POLYNOMIAL, N=n ( $n \leq 6$ )
HYPERELASTIC, VAN DER WAALS
HYPERELASTIC, YEOH

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Coefficients and Strain energy potential: Arruda-Boyce, Mooney-Rivlin, Neo Hooke, Ogden, Polynomial, Reduced Polynomial, Van der Waals, or Yeoh

Using Test Data to Calibrate Material Coefficients

The material coefficients of the hyperelastic models can be calibrated by Abaqus from experimental stress-strain data. In the case of the Marlow and Valanis-Landel models, the test data directly characterize the strain energy potential (there are no material coefficients for these models); these models are described in detail below. The value of N and experimental stress-strain data can be specified for up to four simple tests: uniaxial, equibiaxial, planar, and, if the material is compressible, a volumetric compression test. Abaqus will then compute the material parameters. The material constants are determined through a least-squares-fit procedure, which minimizes the relative error in stress. For the n nominal-stress–nominal-strain data pairs, the relative error measure E is minimized, where

$E = \overset{n}{\sum_{i = 1}} {(1 - T_{i}^{th} / T_{i}^{test})}^{2} .$

$T_{i}^{test}$ is a stress value from the test data, and $T_{i}^{th}$ comes from one of the nominal stress expressions derived below (see “Experimental tests”). Abaqus minimizes the relative error rather than an absolute error measure since this provides a better fit at lower strains. This method is available for all strain energy potentials and any order of N except for the polynomial form, where a maximum of $N = 2$ is allowed. The polynomial models are linear in terms of the constants $C_{i j}$ ; therefore, a linear least-squares procedure can be used. The Arruda-Boyce, Ogden, and Van der Waals potentials are nonlinear in some of their coefficients, thus necessitating the use of a nonlinear least-squares procedure. Fitting of hyperelastic and hyperfoam constants contains a detailed derivation of the related equations.

It is generally best to obtain data from several experiments involving different kinds of deformation over the range of strains of interest in the actual application and to use all of these data to determine the parameters. This is particularly true for the phenomenological models; i.e., the Ogden and the polynomial models. It has been observed that to achieve good accuracy and stability, it is necessary to fit these models using test data from more than one deformation state. In some cases, especially at large strains, removing the dependence on the second invariant may alleviate this limitation. The Arruda-Boyce, neo-Hookean, and Van der Waals models with $β$ = 0 offer a physical interpretation and provide a better prediction of general deformation modes when the parameters are based on only one test. An extensive discussion of this topic can be found in Hyperelastic material behavior.

This method does not allow the hyperelastic properties to be temperature dependent. However, if temperature-dependent test data are available, several curve fits can be conducted by performing a data check analysis on a simple input file. The temperature-dependent coefficients determined by Abaqus can then be entered directly in the actual analysis run.

Optionally, the parameter $β$ in the Van der Waals model can be set to a fixed value while the other parameters are found using a least-squares curve fit.

As many data points as required can be entered from each test. It is recommended that data from all four tests (on samples taken from the same piece of material) be included and that the data points cover the range of nominal strains expected to arise in the actual loading. For the (general) polynomial and Ogden models and for the coefficient $β$ in the Van der Waals model, the planar test data must be accompanied by the uniaxial test data, the biaxial test data, or both of these types of test data; otherwise, the solution to the least-squares fit will not be unique.

The strain data should be given as nominal strain values (change in length per unit of original length). For the uniaxial, equibiaxial, and planar tests stress data are given as nominal stress values (force per unit of original cross-sectional area). These tests allow for entering both compression and tension data. Compressive stresses and strains are entered as negative values.

If compressibility is to be specified, the $D_{i}$ or D can be computed from volumetric compression test data. Alternatively, compressibility can be defined by specifying a Poisson's ratio, in which case Abaqus computes the bulk modulus from the initial shear modulus. If no such data are given, Abaqus/Standard assumes that D or all of the $D_{i}$ are zero, whereas Abaqus/Explicit assumes compressibility corresponding to a Poisson's ratio of 0.475 (see “Compressibility in Abaqus/Explicit” above). For these compression tests the stress data are given as pressure values.

Input File Usage

Use one of the following options to select the strain energy potential:

HYPERELASTIC, TEST DATA INPUT, ARRUDA-BOYCE
HYPERELASTIC, TEST DATA INPUT, MOONEY-RIVLIN
HYPERELASTIC, TEST DATA INPUT, NEO HOOKE
HYPERELASTIC, TEST DATA INPUT, OGDEN, N=n ( $n \leq 6$ )
HYPERELASTIC, TEST DATA INPUT, POLYNOMIAL, N=n ( $n \leq 2$ )
HYPERELASTIC, TEST DATA INPUT, REDUCED POLYNOMIAL, 
N=n ( $n \leq 6$ )
HYPERELASTIC, TEST DATA INPUT, VAN DER WAALS
HYPERELASTIC, TEST DATA INPUT, VAN DER WAALS, 
BETA= $β$  ( $0 \leq β \leq 1$ )
HYPERELASTIC, TEST DATA INPUT, YEOH

In addition, use at least one and up to four of the following options to give the test data (see “Experimental tests” below):

UNIAXIAL TEST DATA
BIAXIAL TEST DATA
PLANAR TEST DATA
VOLUMETRIC TEST DATA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Strain energy potential: Arruda-Boyce, Mooney-Rivlin, Neo Hooke, Ogden, Polynomial, Reduced Polynomial, Van der Waals (Beta: Fitted value or Specify), or Yeoh

In addition, use at least one and up to four of the following options to give the test data (see “Experimental tests” below):

Test DataUniaxial Test Data
Test DataBiaxial Test Data
Test DataPlanar Test Data
Test DataVolumetric Test Data

Alternatively, you can select Strain energy potential: Unknown to define the material temporarily without specifying a particular strain energy potential. Then select MaterialEvaluate to have Abaqus/CAE evaluate the material to determine the optimal strain energy potential.

Specifying the Marlow Model

The Marlow model assumes that the strain energy potential is independent of the second deviatoric invariant ${\bar{I}}_{2}$ . This model is defined by providing test data that define the deviatoric behavior, and, optionally, the volumetric behavior if compressibility must be taken into account. Abaqus will construct a strain energy potential that reproduces the test data exactly, as shown in Figure 1.

The interpolation and extrapolation of stress-strain data with the Marlow model is approximately linear for small and large strains. For intermediate strains in the range 0.1 to 1.0 a noticeable degree of nonlinearity may be observed in the interpolation/extrapolation with the Marlow model; for example, some nonlinearity is apparent between the 4th and 5th data points in Figure 1. To minimize undesirable nonlinearity, make sure that enough data points are specified in the intermediate strain range.

The deviatoric behavior is defined by specifying uniaxial, biaxial, or planar test data. Generally, you can specify either the data from tension tests or the data from compression tests because the tests are equivalent (see Equivalent Experimental Tests). However, for beams, trusses, and rebars, the data from tension and compression tests can be specified together. Volumetric behavior is defined by using one of the following three methods:

Specify nominal lateral strains, in addition to nominal stresses and nominal strains, as part of the uniaxial, biaxial, or planar test data.
Specify Poisson's ratio for the hyperelastic material.
Specify volumetric test data directly. Both hydrostatic tension and hydrostatic compression data can be specified. If only hydrostatic compression data are available, as is usually the case, Abaqus will assume that the hydrostatic pressure is an antisymmetric function of the nominal volumetric strain, $ϵ_{v o l} = J_{v o l} - 1$ .

If you do not define volumetric behavior, Abaqus/Standard assumes fully incompressible behavior, while Abaqus/Explicit assumes compressibility corresponding to a Poisson's ratio of 0.475.

Material test data in which the stress does not vary smoothly with increasing strain may lead to convergence difficulty during the simulation. It is highly recommended that smooth test data be used to define the Marlow form. Abaqus provides a smoothing algorithm, which is described in detail later in this section.

The test data for the Marlow model can also be given as a function of temperature and field variables. You must specify the number of user-defined field variable dependencies required.

Uniaxial, biaxial, and planar test data must be given in ascending order of the nominal strains; volumetric test data must be given in descending order of the volume ratio.

Input File Usage

To define the Marlow test data as a function of temperature and/or field variables, use the following option:

HYPERELASTIC,  MARLOW

with one of the following first three options and, optionally, the fourth option:

UNIAXIAL TEST DATA, DEPENDENCIES=n
BIAXIAL TEST DATA, DEPENDENCIES=n
PLANAR TEST DATA, DEPENDENCIES=n
VOLUMETRIC TEST DATA, DEPENDENCIES=n

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Strain energy potential: Marlow

In addition, select one of the following first three options and, optionally, the fourth option to give the test data (see “Experimental tests” below):

Test DataUniaxial Test Data
Test DataBiaxial Test Data
Test DataPlanar Test Data
Test DataVolumetric Test Data

In each of the Test Data Editor dialog boxes, you can toggle on Use temperature-dependent data to define the test data as a function of temperature and/or select the Number of field variables to define the test data as a function of field variables.

Alternatively, you can select Material Evaluate to have Abaqus/CAE evaluate the material. If you included temperature dependencies, field variable dependencies, or lateral nominal strain in the test data—which can only be defined in the Marlow hyperelastic definition—Marlow will be the only strain energy potential available for evaluation.

Specifying the Valanis-Landel Model

In general, the deviatoric part of the strain energy potential of the Valanis-Landel model depends on both the first, ${\bar{I}}_{1}$ , and the second, ${\bar{I}}_{2}$ , deviatoric invariants. You define this model by providing test data and, optionally, the Poisson's ratio. Abaqus constructs a strain energy potential that reproduces the test data exactly.

You define the deviatoric behavior by specifying uniaxial test data. You must specify data from both tension tests and compression tests together for this model. Volumetric behavior is defined by using one of the following methods:

Specify nominal lateral strains, in addition to nominal stresses and nominal strains, as part of the uniaxial test data.
Specify Poisson's ratio for the hyperelastic material.
Specify volumetric test data directly. You can specify both hydrostatic tension and hydrostatic compression data. If only hydrostatic compression data are available, as is usually the case, Abaqus assumes that the hydrostatic pressure is an antisymmetric function of the nominal volumetric strain, $ϵ_{v o l} = J_{v o l} - 1$ .

If a Poisson's ratio of 0.5 is specified, the material behavior is assumed to be fully incompressible in Abaqus/Standard.

Material test data in which the stress does not vary smoothly with increasing strain can lead to convergence difficulty during the simulation. It is highly recommended that you use smooth test data to define the Valanis-Landel form. Abaqus provides a smoothing algorithm, which is described in detail later in this section.

The test data for the Valanis-Landel model can also be given as a function of temperature and field variables. You must specify the number of user-defined field variable dependencies required.

Uniaxial test data must be given in ascending order of the nominal strains.

Input File Usage

To define the Valanis-Landel test data as a function of temperature and/or field variables, use both of the following options:

HYPERELASTIC, VALANIS-LANDEL
UNIAXIAL TEST DATA, DEPENDENCIES=n

and, optionally,

VOLUMETRIC TEST DATA, DEPENDENCIES=n

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Strain energy potential: Valanis-Landel

User Subroutine Specification in Abaqus/Standard

An alternative method provided in Abaqus/Standard for defining the hyperelastic material parameters allows the strain energy potential to be defined in user subroutine UHYPER or in user subroutine UHYPER_STRETCH. You can specify either compressible or incompressible behavior. Optionally, you can specify the number of property values needed as data in the user subroutine. If needed, you can specify the number of solution-dependent variables (see About User Subroutines and Utilities).

User subroutine UHYPER requires that the values of the derivatives of the strain energy density function of the hyperelastic material are defined with respect to the strain invariants.

User subroutine UHYPER_STRETCH assumes that the strain energy potential uses the Valanis-Landel form. It requires that the values of the derivatives of the strain energy density function of the hyperelastic material are defined with respect to the principal deviatoric stretches, ${\bar{λ}}_{i}$ , and elastic volume ratio, $J_{e ℓ}$ .

Input File Usage

Use one of the following options to specify the strain energy potential in user subroutine UHYPER:

HYPERELASTIC, USER, FORMULATION=INVARIANT, TYPE=COMPRESSIBLE, PROPERTIES=n
HYPERELASTIC, USER, FORMULATION=INVARIANT, TYPE=INCOMPRESSIBLE, PROPERTIES=n

Use one of the following options to specify the strain energy potential in user subroutine UHYPER_STRETCH:

HYPERELASTIC, USER, FORMULATION=STRETCH, TYPE=COMPRESSIBLE, PROPERTIES=n
HYPERELASTIC, USER, FORMULATION=STRETCH, TYPE=INCOMPRESSIBLE, PROPERTIES=n

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Coefficients and Strain energy potential: User-defined: optionally, toggle on Include compressibility and/or specify the Number of property values

Experimental Tests

For a homogeneous material, homogeneous deformation modes suffice to characterize the material constants. Abaqus accepts test data from the following deformation modes:

Uniaxial tension and compression
Equibiaxial tension and compression
Planar tension and compression (also known as pure shear)
Volumetric tension and compression

These modes are illustrated schematically in Figure 2 and are described below. The most commonly performed experiments are uniaxial tension, uniaxial compression, and planar tension.

Combine data from these three test types to get a good characterization of the hyperelastic material behavior.

For the incompressible version of the material model, the stress-strain relationships for the different tests are developed using derivatives of the strain energy function with respect to the strain invariants. We define these relations in terms of the nominal stress (the force divided by the original, undeformed area) and the nominal, or engineering, strain defined below.

The deformation gradient, expressed in the principal directions of stretch, is

$F = [\begin{matrix} λ_{1} & 0 & 0 \\ 0 & λ_{2} & 0 \\ 0 & 0 & λ_{3} \end{matrix}],$

where $λ_{1}$ , $λ_{2}$ , and $λ_{3}$ are the principal stretches: the ratios of current length to length in the original configuration in the principal directions of a material fiber. The principal stretches, $λ_{i}$ , are related to the principal nominal strains, $ϵ_{i}$ , by

$λ_{i} = 1 + ϵ_{i} .$

Because we assume incompressibility and isothermal response, $J = \det (F) = 1$ and, hence, $λ_{1} λ_{2} λ_{3}$ = 1. The deviatoric strain invariants in terms of the principal stretches are then

${\bar{I}}_{1} = λ_{1}^{2} + λ_{2}^{2} + λ_{3}^{2},$

and

${\bar{I}}_{2} = λ_{1}^{- 2} + λ_{2}^{- 2} + λ_{3}^{- 2} .$

Uniaxial Tests

The uniaxial deformation mode is characterized in terms of the principal stretches, $λ_{i}$ , as

$λ_{1} = λ_{U}, λ_{2} = λ_{3} = 1 / \sqrt{λ_{U}},$

where $λ_{U}$ is the stretch in the loading direction. The nominal strain is defined by $ε_{U} = λ_{U} - 1.$

To derive the uniaxial nominal stress $T_{U}$ , we invoke the principle of virtual work:

$δ U = T_{U} δ λ_{U},$

so that

$T_{U} = \frac{\partial U}{\partial λ_{U}} = 2 (1 - λ_{U}^{- 3}) (λ_{U} \frac{\partial U}{\partial {\bar{I}}_{1}} + \frac{\partial U}{\partial {\bar{I}}_{2}}) .$

The uniaxial tension test is the most common of all the tests and is usually performed by pulling a “dog-bone” specimen. The uniaxial compression test is performed by loading a compression button between lubricated surfaces. The loading surfaces are lubricated to minimize any barreling effect in the button that would cause deviations from a homogeneous uniaxial compression stress-strain state.

Input File Usage

UNIAXIAL TEST DATA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Test DataUniaxial Test Data

Equibiaxial Tests

The equibiaxial deformation mode is characterized in terms of the principal stretches, $λ_{i}$ , as

$λ_{1} = λ_{2} = λ_{B}, λ_{3} = 1 / λ_{B}^{2},$

where $λ_{B}$ is the stretch in the two perpendicular loading directions. The nominal strain is defined by $ε_{B} = λ_{B} - 1.$

To develop the expression for the equibiaxial nominal stress, $T_{B}$ , we again use the principle of virtual work (assuming that the stress perpendicular to the loading direction is zero),

$δ U = 2 T_{B} δ λ_{B},$

so that

$T_{B} = \frac{1}{2} \frac{\partial U}{\partial λ_{B}} = 2 (λ_{B} - λ_{B}^{- 5}) (\frac{\partial U}{\partial {\bar{I}}_{1}} + λ_{B}^{2} \frac{\partial U}{\partial {\bar{I}}_{2}}) .$

In practice, the equibiaxial compression test is rarely performed because of experimental setup difficulties. In addition, this deformation mode is equivalent to a uniaxial tension test, which is straightforward to conduct.

A more common test is the equibiaxial tension test, in which a stress state with two equal tensile stresses and zero shear stress is created. This state is usually achieved by stretching a square sheet in a biaxial testing machine. It can also be obtained by inflating a circular membrane into a spheroidal shape (like blowing up a balloon). The stress field in the middle of the membrane then closely approximates equibiaxial tension, provided that the thickness of the membrane is very much smaller than the radius of curvature at this point. However, the strain distribution will not be quite uniform, and local strain measurements will be required. Once the strain and radius of curvature are known, the nominal stress can be derived from the inflation pressure.

Input File Usage

BIAXIAL TEST DATA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Test DataBiaxial Test Data

Planar Tests

The planar deformation mode is characterized in terms of the principal stretches, $λ_{i}$ , as

$λ_{1} = λ_{S}, λ_{2} = 1, λ_{3} = 1 / λ_{S},$

where $λ_{S}$ is the stretch in the loading direction. Then, the nominal strain in the loading direction is $ε_{S} = λ_{S} - 1.$

This test is also called a “pure shear” test since, in terms of logarithmic strains,

$ε_{1} = \ln λ_{1} = - \ln λ_{3} = - ε_{3}, ε_{2} = \ln λ_{2} = 0,$

which corresponds to a state of pure shear at an angle of 45° to the loading direction.

The principle of virtual work gives

$δ U = T_{S} δ λ_{S},$

where $T_{S}$ is the nominal planar stress, so that

$T_{S} = \frac{\partial U}{\partial λ_{S}} = 2 (λ_{S} - λ_{S}^{- 3}) (\frac{\partial U}{\partial {\bar{I}}_{1}} + \frac{\partial U}{\partial {\bar{I}}_{2}}) .$

For the (general) polynomial and Ogden models and for the coefficient $β$ in the Van der Waals model this equation alone will not determine the constants uniquely. The planar test data must be augmented by uniaxial test data and/or biaxial test data to determine the material parameters.

Planar tests are usually done with a thin, short, and wide rectangular strip of material fixed on its wide edges to rigid loading clamps that are moved apart. If the separation direction is the 1-direction and the thickness direction is the 3-direction, the comparatively long size of the specimen in the 2-direction and the rigid clamps allow us to use the approximation $λ_{2} = 1$ ; that is, there is no deformation in the wide direction of the specimen. This deformation mode could also be called planar compression if the 3-direction is considered to be the primary direction. All forms of incompressible plane strain behavior are characterized by this deformation mode. Consequently, if plane strain analysis is performed, planar test data represent the relevant form of straining of the material.

Input File Usage

PLANAR TEST DATA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Test DataPlanar Test Data

Volumetric Tests

The following discussion describes procedures for obtaining $D_{i}$ values (or D, for the Arruda-Boyce and Van der Waals models) corresponding to the actual material behavior. With these values you can compare the material's initial bulk modulus, $K_{0} = 2 / D_{1}$ , to its initial shear modulus ( $μ_{0} = 2 (C_{10} + C_{01})$ for the polynomial model, $μ_{0} = \sum_{i = 1}^{N} μ_{i}$ for Ogden's model) and then judge whether $D_{i}$ values that will provide results are sufficiently realistic. For Abaqus/Explicit caution should be used; $K_{0} / μ_{0}$ should be less than 100. Otherwise, noisy solutions will be obtained and time increments will be excessively small (see “Compressibility in Abaqus/Explicit” above). The $D_{i}$ and D can be calculated from data obtained in pure volumetric compression of a specimen (volumetric tension tests are much more difficult to perform). In a pure volumetric test $λ_{1} = λ_{2} = λ_{3} = λ_{V}$ ; therefore, ${\bar{I}}_{1} = {\bar{I}}_{2} = 3$ and $J = λ_{V}^{3} = V / V_{0}$ (the volume ratio). Using the polynomial form of the strain energy potential, the total pressure stress on the specimen is obtained as

$p = - (\frac{σ_{1} + σ_{2} + σ_{3}}{3}) = - \overset{N}{\sum_{i = 1}} 2 i \frac{1}{D_{i}} {(λ_{V}^{3} - 1)}^{2 i - 1} .$

This equation can be used to determine the $D_{i}$ . If we are using a second-order polynomial series for U, we have $N = 2$ , and so two $D_{i}$ are needed. Therefore, a minimum of two points on the pressure-volume ratio curve are required to give two equations for the $D_{i}$ . For the Ogden and reduced polynomial potentials $D_{i}$ can be determined for up to $N = 6$ . A linear least-squares fit is performed when more than N data points are provided.

An approximate way of conducting a volumetric test consists of using a cylindrical rubber specimen that fits snugly inside a rigid container and whose top surface is compressed by a rigid piston. Although both volumetric and deviatoric deformation are present, the deviatoric stresses will be several orders of magnitude smaller than the hydrostatic stresses (because the bulk modulus is much higher than the shear modulus) and can be neglected. The compressive stress imposed by the rigid piston is effectively the pressure, and the volumetric strain in the rubber cylinder is computed from the piston displacement.

Nonzero values of $D_{i}$ affect the uniaxial, equibiaxial, and planar stress results. However, since the material is assumed to be only slightly compressible, the techniques described for obtaining the deviatoric coefficients should give sufficiently accurate values even though they assume that the material is fully incompressible.

Input File Usage

VOLUMETRIC TEST DATA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Test DataVolumetric Test Data

Equivalent Experimental Tests

The superposition of a tensile or compressive hydrostatic stress on a loaded, fully incompressible elastic body results in different stresses but does not change the deformation. Thus, Figure 3 shows that some apparently different loading conditions are actually equivalent in their deformations and, therefore, are equivalent tests:

Uniaxial tension $⟺$ Equibiaxial compression
Uniaxial compression $⟺$ Equibiaxial tension
Planar tension $⟺$ Planar compression

On the other hand, the tensile and compressive cases of the uniaxial and equibiaxial modes are independent from each other: uniaxial tension and uniaxial compression provide independent data.

Smoothing the Test Data

Experimental test data often contain noise in the sense that the test variable is both slowly varying and also corrupted by random noise. This noise can affect the quality of the strain energy potential that Abaqus derives. This noise is particularly a problem with the Marlow form, where a strain energy potential that exactly describes the test data that are used to calibrate the model is computed. It is less of a concern with the other forms, since smooth functions are fitted through the test data.

Abaqus provides a smoothing technique to remove the noise from the test data based on the Savitzky-Golay method. The idea is to replace each data point by a local average of its surrounding data points, so that the level of noise can be reduced without biasing the dominant trend of the test data. In the implementation a cubic polynomial is fitted through each data point i and n data points to the immediate left and right of that point. A least-squares method is used to fit the polynomial through these $2 n + 1$ points. The value of data point i is then replaced by the value of the polynomial at the same position. Each polynomial is used to adjust one data point except near the ends of the curve, where a polynomial is used to adjust multiple points, because the first and last few points cannot be the center of the fitting set of data points. This process is applied repeatedly to all data points until two consecutive passes through the data produce nearly the same results.

By default, the test data are not smoothed. If smoothing is specified, the default value is n=3. Alternatively, you can specify the number of data points to the left and right of a data point in the moving window within which a least-squares polynomial is fit.

Input File Usage

For the Marlow form, use one of the first three options and, optionally, the fourth option; for the Valanis-Landel model, use the first option and, optionally, the fourth option; and for the other potential forms, use one and up to four of the following options:

UNIAXIAL TEST DATA,  SMOOTH=n ( $n \geq 2$ )
BIAXIAL TEST DATA,  SMOOTH=n ( $n \geq 2$ )
PLANAR TEST DATA,  SMOOTH=n ( $n \geq 2$ )
VOLUMETRIC TEST DATA,  SMOOTH=n ( $n \geq 2$ )

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityHyperelastic: 
Material type: Isotropic; Input source: Test data and Test DataUniaxial Test Data, Biaxial Test Data, Planar Test Data, or Volumetric Test Data

In each of the Test Data Editor dialog boxes, toggle on Apply smoothing, and select a value for n ( $n \geq 2$ ).

Model Prediction of Material Behavior Versus Experimental Data

Once the strain energy potential is determined, the behavior of the hyperelastic model in Abaqus is established. However, the quality of this behavior must be assessed: the prediction of material behavior under different deformation modes must be compared against the experimental data. You must judge whether the strain energy potentials determined by Abaqus are acceptable, based on the correlation between the Abaqus predictions and the experimental data. You can evaluate the hyperelastic behavior automatically in Abaqus/CAE. Alternatively, single-element test cases can be used to derive the nominal stress–nominal strain response of the material model.

See Fitting of rubber test data, which illustrates the entire process of fitting hyperelastic constants to a set of test data.

Hyperelastic Material Stability

An important consideration in judging the quality of the fit to experimental data is the concept of material or Drucker stability. Abaqus checks the Drucker stability of the material for the first three deformation modes described above.

The Drucker stability condition for an incompressible material requires that the change in the stress, $d σ$ , following from any infinitesimal change in the logarithmic strain, $d ε$ , satisfies the inequality

$d σ : d ε > 0.$

Using $d σ = D : d ε$ , where $D$ is the tangent material stiffness, the inequality becomes

$d ε : D : d ε > 0,$

thus requiring the tangential material stiffness to be positive-definite.

For an isotropic elastic formulation the inequality can be represented in terms of the principal stresses and strains,

$d σ_{1} d ε_{1} + d σ_{2} d ε_{2} + d σ_{3} d ε_{3} > 0.$

As before, since the material is assumed to be incompressible, we can choose any value for the hydrostatic pressure without affecting the strains. A convenient choice for the stability calculation is $σ_{3} = d σ_{3} = 0$ , which allows us to ignore the third term in the above equation.

The relation between the changes in stress and in strain can then be obtained in the form of the matrix

$(\begin{matrix} d σ_{1} \\ d σ_{2} \end{matrix}) = (\begin{matrix} D_{11} & D_{12} \\ D_{21} & D_{22} \end{matrix}) (\begin{matrix} d ε_{1} \\ d ε_{2} \end{matrix}),$

where $D_{i j} = D_{i j} (λ_{1}, λ_{2}, λ_{3})$ . For material stability $D$ must be positive-definite; thus, it is necessary that

$D_{11} + D_{22} > 0,$

$D_{11} D_{22} - D_{12} D_{21} > 0.$

This stability check is performed for the polynomial models, the Ogden potential, the Van der Waals form, the Marlow form, and the Valanis-Landel form. The Arruda-Boyce form is always stable for positive values of ( $μ$ , $λ_{m}$ ); hence, it suffices to check the material coefficients to ensure stability.

You should be careful when defining the $C_{i j}$ or $(μ_{i}, α_{i})$ for the polynomial models or the Ogden form: especially when $N > 1$ , the behavior at higher strains is strongly sensitive to the values of the $C_{i j}$ or $(μ_{i}, α_{i})$ , and unstable material behavior may result if these values are not defined correctly. When some of the coefficients are strongly negative, instability at higher strain levels is likely to occur.

Abaqus performs a check on the stability of the material for six different forms of loading—uniaxial tension and compression, equibiaxial tension and compression, and planar tension and compression—for $0.1 \leq λ_{1} \leq 10.0$ (nominal strain range of $- 0.9 \leq ϵ_{1} \leq 9.0$ ) at intervals $Δ λ_{1} = 0.01$ . If an instability is found, Abaqus issues a warning message and prints the lowest absolute value of $ϵ_{1}$ for which the instability is observed. Ideally, no instability occurs. If instabilities are observed at strain levels that are likely to occur in the analysis, it is strongly recommended that you either change the material model or carefully examine and revise the material input data. If user subroutine UHYPER or user subroutine UHYPER_STRETCH is used to define the hyperelastic material, you are responsible for ensuring stability.

Improving the Accuracy and Stability of the Test Data Fit

Unfortunately, the initial fit of the models to experimental data may not come out as well as expected. This is particularly true for the most general models, such as the (general) polynomial model and the Ogden model. For some of the simpler models, stability is assured by following some simple rules.

For positive values of the initial shear modulus, $μ$ , and the locking stretch, $λ_{m}$ , the Arruda-Boyce form is always stable.
For positive values of the coefficient $C_{10}$ the neo-Hookean form is always stable.
Given positive values of the initial shear modulus, $μ$ , and the locking stretch, $λ_{m}$ , the stability of the Van der Waals model depends on the global interaction parameter, a.
For the Yeoh model stability is assured if all $C_{i 0} > 0$ . Typically, however, $C_{20}$ will be negative, since this helps capture the S-shape feature of the stress-strain curve. Thus, reducing the absolute value of $C_{20}$ or magnifying the absolute value of $C_{10}$ will help make the Yeoh model more stable.

In all cases the following suggestions may improve the quality of the fit:

Both tension and compression data are allowed; compressive stresses and strains are entered as negative values. Use compression or tension data depending on the application: it is difficult to fit a single material model accurately to both tensile and compressive data.
Always use many more experimental data points than unknown coefficients.
If $N \geq 3$ is used, experimental data should be available to at least 100% tensile strain or 50% compressive strain.
Perform different types of tests (e.g., compression and simple shear tests). Proper material behavior for a deformation mode requires test data to characterize that mode.
Check for warning messages about material instability or error messages about lack of convergence in fitting the test data. This check is especially important with new test data; a simple finite element model with the new test data can be run through the analysis input file processor to check the material stability.
Use the material evaluation capability in Abaqus/CAE to compare the response curves for different strain energy potentials to the experimental data. Alternatively, you can perform one-element simulations for simple deformation modes and compare the Abaqus results against the experimental data. The X–Y plotting options in the Visualization module of Abaqus/CAE can be used for this comparison.
Delete some data points at very low strains if large strains are anticipated. A disproportionate number of low strain points may unnecessarily bias the accuracy of the fit toward the low strain range and cause greater errors in the large strain range.
Delete some data points at the highest strains if small to moderate strains are expected. The high strain points may force the fitting to lose accuracy and/or stability in the low strain range.
Pick data points at evenly spaced strain intervals over the expected range of strains, which will result in similar accuracy throughout the entire strain range.
The higher the order of N, the more oscillations are likely to occur, leading to instabilities in the stress-strain curves. If the (general) polynomial model is used, lower the order of N from 2 to 1 (3 to 2 for Ogden), especially if the maximum strain level is low (say, less than 100% strain).
If multiple types of test data are used and the fit still comes out poorly, some of the test data probably contain experimental errors. New tests may be needed. One way of determining which test data are erroneous is to first calibrate the initial shear modulus $μ_{0}^{t e s t}$ of the material. Then fit each type of test data separately in Abaqus and compute the shear modulus, $μ_{0}^{f i t}$ , from the material constants using the relations
$μ_{0}^{f i t} = 2 (C_{10} + C_{01}) (polynomial form) or μ_{0}^{f i t} = \sum_{i = 1}^{N} μ_{i} (Ogden form) .$

Alternatively, the initial Young's modulus, $E_{0}^{t e s t}$ , can be calibrated and compared with
$E_{0}^{f i t} = 6 (C_{10} + C_{01}) (polynomial form) or E_{0}^{f i t} = 3 \sum_{i = 1}^{N} μ_{i} (Ogden form) .$

The values of $μ_{0}^{f i t}$ or $E_{0}^{f i t}$ that are most different from $μ_{0}^{t e s t}$ or $E_{0}^{t e s t}$ indicate the erroneous test data.

Elements

The hyperelastic material model can be used with solid (continuum) elements, finite-strain shells (except S4), continuum shells, membranes, and one-dimensional elements (trusses and rebars). In Abaqus/Standard the hyperelastic material model can be also used with Timoshenko beams (B21, B22, B31, B31OS, B32, B32OS, PIPE21, PIPE22, PIPE31, PIPE32, and their “hybrid” equivalents). It cannot be used with Euler-Bernoulli beams (B23, B23H, B33, and B33H) and small-strain shells (STRI3, STRI65, S4R5, S8R, S8R5, S9R5).

Pure Displacement Formulation Versus Hybrid Formulation in Abaqus/Standard

For continuum elements in Abaqus/Standard hyperelasticity can be used with the pure displacement formulation elements or with the “hybrid” (mixed formulation) elements. Because elastomeric materials are usually almost incompressible, fully integrated pure displacement method elements are not recommended for use with this material, except for plane stress cases. If fully or selectively reduced-integration displacement method elements are used with the almost incompressible form of this material model, a penalty method is used to impose the incompressibility constraint in anything except plane stress analysis. The penalty method can sometimes lead to numerical difficulties; therefore, the fully or selectively reduced-integrated “hybrid” formulation elements are recommended for use with hyperelastic materials.

In general, an analysis using a single hybrid element will be only slightly more computationally expensive than an analysis using a regular displacement-based element. However, when the wavefront is optimized, the Lagrange multipliers may not be ordered independently of the regular degrees of freedom associated with the element. Thus, the wavefront of a very large mesh of second-order hybrid tetrahedra may be noticeably larger than that of an equivalent mesh using regular second-order tetrahedra. This may lead to significantly higher CPU costs, disk space, and memory requirements.

Incompatible Mode Elements in Abaqus/Standard

Incompatible mode elements should be used with caution in applications involving large strains. Convergence may be slow, and in hyperelastic applications inaccuracies may accumulate. Erroneous stresses may sometimes appear in incompatible mode hyperelastic elements that are unloaded after having been subjected to a complex deformation history.

Procedures

Hyperelasticity must always be used with geometrically nonlinear analyses (General and Perturbation Procedures).