Anisotropic Hyperelastic Behavior

In this case the strain energy function is expressed directly in terms of the components of a suitable strain tensor, such as the Green strain tensor (see Strain measures):

where ${\mathit{\epsilon }}^G=\frac{1}{2}\left(\mathbf{C}-\mathbf{I}\right)$ is Green's strain; $\mathbf{C}={\mathbf{F}}^T\cdot \mathbf{F}$ is the right Cauchy-Green strain tensor; $\mathbf{F}$ is the deformation gradient; and $\mathbf{I}$ is the identity matrix. Without loss of generality, the strain energy function can be written in the form

where ${\overline{\mathit{\epsilon }}}^G=\frac{1}{2}\left(\overline{\mathbf{C}}-\mathbf{I}\right)$ is the modified Green strain tensor; $\overline{C}=J^{-\frac{2}{3}}\mathbf{C}$ is the distortional part of the right Cauchy-Green strain; $J=det\left(\mathbf{F}\right)$ is the total volume change; and $J^{e\mathrm{\ell }}$ is the elastic volume ratio as defined below in Thermal Expansion.

The underlying assumption in models based on the strain-based formulation is that the preferred material directions are initially aligned with an orthogonal coordinate system in the reference (stress-free) configuration. These directions may become non-orthogonal only after deformation. Examples of this form of strain energy function include the generalized Fung-type form described below.

Using the continuum theory of fiber-reinforced composites (Spencer, 1984) the strain energy function can be expressed directly in terms of the invariants of the deformation tensor and fiber directions. For example, consider a composite material that consists of an isotropic hyperelastic matrix reinforced with $N$ families of fibers. The directions of the fibers in the reference configuration are characterized by a set of unit vectors ${\mathbf{A}}_{\alpha }$, ($\alpha =1,\mathrm{\dots },N$). Assuming that the strain energy depends not only on deformation, but also on the fiber directions, the following form is postulated

The strain energy of the material must remain unchanged if both matrix and fibers in the reference configuration undergo a rigid body rotation. Then, following Spencer (1984), the strain energy can be expressed in terms of an irreducible set of scalar invariants that form the integrity basis of the tensor $\mathbf{C}$ and the vectors ${\mathbf{A}}_{\alpha }$:

where ${\overline{I}}_1$ and ${\overline{I}}_2$ are the first and second deviatoric strain invariants; $J^{e\mathrm{\ell }}$ is the elastic volume ratio (or third strain invariant); ${\overline{I}}_{4\left(\alpha \beta \right)}$ and ${\overline{I}}_{5\left(\alpha \beta \right)}$ are the pseudo-invariants of $\overline{\mathbf{C}}$, ${\mathbf{A}}_{\alpha }$; and ${\mathbf{A}}_{\beta }$, defined as:

The terms ${\zeta }_{\alpha \beta }$ are geometrical constants (independent of deformation) equal to the cosine of the angle between the directions of any two families of fibers in the reference configuration:

Unlike for the case of the strain-based formulation, in the invariant-based formulation the fiber directions need not be orthogonal in the initial configuration. An example of an invariant-based energy function is the form proposed by Holzapfel, Gasser, and Ogden (2000) for arterial walls (see Holzapfel-Gasser-Ogden Form below).

The generalized Fung strain energy potential has the following form:

where U is the strain energy per unit of reference volume; $c$ and D are temperature-dependent material parameters; $J^{e\mathrm{\ell }}$ is the elastic volume ratio as defined below in Thermal Expansion; and $Q$ is defined as

where $b_{ijkl}$ is a dimensionless symmetric fourth-order tensor of anisotropic material constants that can be temperature dependent and ${\overline{\epsilon }}_{ij}^G$ are the components of the modified Green strain tensor.

The initial deviatoric elasticity tensor, ${\overline{\mathbf{D}}}_0$, and bulk modulus, $K_0$, are given by

Abaqus supports two forms of the generalized Fung model: fully anisotropic and orthotropic. The number of independent components $b_{ijlk}$ that must be specified depends on the level of anisotropy of the material: 21 for the fully anisotropic case and 9 for the orthotropic case.

The form of the strain energy potential is based on that proposed by Holzapfel, Gasser, and Ogden (2000) and Gasser, Ogden, and Holzapfel (2006) for modeling arterial layers with distributed collagen fiber orientations:

with

where U is the strain energy per unit of reference volume; $C_{10}$, D, $k_1$, $k_2$, and $\kappa$ are temperature-dependent material parameters; $N$ is the number of families of fibers ($N\le 3$); ${\overline{I}}_1$ is the first deviatoric strain invariant; $J^{e\mathrm{\ell }}$ is the elastic volume ratio as defined below in Thermal Expansion; and ${\overline{I}}_{4\left(\alpha \alpha \right)}$ are pseudo-invariants of $\overline{\mathbf{C}}$ and ${\mathbf{A}}_{\alpha }$.

The model assumes that the directions of the collagen fibers within each family are dispersed (with rotational symmetry) about a mean preferred direction. The parameter $\kappa$ ($0\le \kappa \le 1/3$) describes the level of dispersion in the fiber directions. If $\rho \left(\mathrm{\Theta }\right)$ is the orientation density function that characterizes the distribution (it represents the normalized number of fibers with orientations in the range $\left[\mathrm{\Theta },\mathrm{\Theta }+d\mathrm{\Theta }\right]$ with respect to the mean direction), the parameter $\kappa$ is defined as

It is also assumed that all families of fibers have the same mechanical properties and the same dispersion. When $\kappa =0,$ the fibers are perfectly aligned (no dispersion). When $\kappa =1/3,$ the fibers are randomly distributed and the material becomes isotropic; this corresponds to a spherical orientation density function.

The strain-like quantity ${\overline{E}}_{\alpha }$ characterizes the deformation of the family of fibers with mean direction ${\mathbf{A}}_{\alpha }$. For perfectly aligned fibers ($\kappa =0$), ${\overline{E}}_{\alpha }={\overline{I}}_{4\left(\alpha \alpha \right)}-1$; and for randomly distributed fibers ($\kappa =1/3$), ${\overline{E}}_{\alpha }=\left({\overline{I}}_1-3\right)/3$.

The first two terms in the expression of the strain energy function represent the distortional and volumetric contributions of the non-collagenous isotropic ground material, and the third term represents the contributions from the different families of collagen fibers, taking into account the effects of dispersion. A basic assumption of the model is that collagen fibers can support tension only, because they would buckle under compressive loading. Thus, the anisotropic contribution in the strain energy function appears only when the strain of the fibers is positive or, equivalently, when ${\overline{E}}_{\alpha }>0$. This condition is enforced by the term $⟨{\overline{E}}_{\alpha }⟩$, where the operator $⟨\cdot ⟩$ stands for the Macauley bracket and is defined as $⟨x⟩=\frac{1}{2}\left(\left|x\right|+x\right)$.

See Anisotropic hyperelastic modeling of arterial layers for an example of an application of the Holzapfel-Gasser-Ogden energy potential to model arterial layers with distributed collagen fiber orientation.

The initial deviatoric elasticity tensor, ${\overline{\mathbf{D}}}_0$, and bulk modulus, $K_0$, are given by

where $\mathrm{\Im }$ is the fourth-order unit tensor, and $H\left(x\right)$ is the Heaviside unit step function.

Alternatively, you can define the form of a strain-based strain energy potential directly with user subroutine UANISOHYPER_STRAIN in Abaqus/Standard or VUANISOHYPER_STRAIN in Abaqus/Explicit. The derivatives of the strain energy potential with respect to the components of the modified Green strain and the elastic volume ratio, $J^{e\mathrm{\ell }}$, must be provided directly through these user subroutines.

Either compressible or incompressible behavior can be specified in Abaqus/Standard; only nearly incompressible behavior is allowed in Abaqus/Explicit.

Optionally, you can specify the number of property values needed as data in the user subroutine as well as the number of solution-dependent variables (see About User Subroutines and Utilities).

Alternatively, you can define the form of an invariant-based strain energy potential directly with user subroutine UANISOHYPER_INV in Abaqus/Standard or VUANISOHYPER_INV in Abaqus/Explicit. Either compressible or incompressible behavior can be specified in Abaqus/Standard; only nearly incompressible behavior is allowed in Abaqus/Explicit.

Optionally, you can specify the number of property values needed as data in the user subroutine and the number of solution-dependent variables (see About User Subroutines and Utilities).

The derivatives of the strain energy potential with respect to the strain invariants must be provided directly through user subroutine UANISOHYPER_INV in Abaqus/Standard and VUANISOHYPER_INV in Abaqus/Explicit.

In Abaqus/Standard the use of “hybrid” (mixed formulation) elements is required for incompressible materials. In plane stress, shell, and membrane elements the material is free to deform in the thickness direction. In this case special treatment of the volumetric behavior is not necessary; the use of regular stress/displacement elements is satisfactory.

With the exception of the plane stress and one-dimensional 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, some compressibility must be modeled. The difficulty is that, in many cases, the actual material behavior provides too little compressibility for the algorithms to work efficiently. Thus, except for the plane stress case, 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. Failing to provide enough compressibility may introduce high frequency noise into the dynamic solution and require the use of excessively small time increments. 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 of the anisotropic hyperelastic model, by default Abaqus/Explicit assumes the value $K_0/{\mu }_0=20$, where ${\mu }_0$ is the largest value of the initial shear modulus (among the different material directions). The exception is for the case of user-defined forms, where some compressibility must be defined directly within user subroutine UANISOHYPER_INV or VUANISOHYPER_INV.