Linear Elastic Behavior

The total stress is defined from the total elastic strain as

where $\mathit{\sigma }$ is the total stress (“true,” or Cauchy stress in finite-strain problems), ${\mathbf{D}}^{el}$ is the fourth-order elasticity tensor, and ${\mathit{\epsilon }}^{el}$ is the total elastic strain (log strain in finite-strain problems). Do not use the linear elastic material definition when the elastic strains might become large; use a hyperelastic model instead. Even in finite-strain problems the elastic strains should still be small (less than 5%).

Depending on the number of symmetry planes for the elastic properties, a material can be classified as either isotropic (an infinite number of symmetry planes passing through every point) or anisotropic (no symmetry planes). Some materials have a restricted number of symmetry planes passing through every point; for example, orthotropic materials have two orthogonal symmetry planes for the elastic properties. The number of independent components of the elasticity tensor ${\mathbf{D}}^{el}$ depends on such symmetry properties. You define the level of anisotropy and method of defining the elastic properties, as described below. If the material is anisotropic, a local orientation (Orientations) must be used to define the direction of anisotropy.

Linear elastic materials must satisfy the conditions of material or Drucker stability (see the discussion on material stability in Hyperelastic Behavior of Rubberlike Materials). Stability requires that the tensor ${\mathbf{D}}^{el}$ be positive definite, which leads to certain restrictions on the values of the elastic constants. The stress-strain relations for several different classes of material symmetries are given below. The appropriate restrictions on the elastic constants stemming from the stability criterion are also given.

The simplest form of linear elasticity is the isotropic case, and the stress-strain relationship is given by

The elastic properties are completely defined by giving the Young's modulus, E, and the Poisson's ratio, $\nu$ . The shear modulus, G, can be expressed in terms of E and $\nu$ as $G=E/2\left(1+\nu \right)$ . These parameters can be given as functions of temperature and of other predefined fields, if necessary.

In Abaqus/Standard spatially varying isotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (Distribution Definition). The distribution must include default values for E and $\nu$ . If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

Linear elasticity in an orthotropic material is most easily defined by giving the “engineering constants”: the three moduli $E_1$ , $E_2$ , $E_3$ ; Poisson's ratios ${\nu }_{12}$ , ${\nu }_{13}$ , ${\nu }_{23}$ ; and the shear moduli $G_{12}$ , $G_{13}$ , and $G_{23}$ associated with the material's principal directions. These moduli define the elastic compliance according to

The quantity ${\nu }_{ij}$ has the physical interpretation of the Poisson's ratio that characterizes the transverse strain in the j-direction, when the material is stressed in the i-direction. In general, ${\nu }_{ij}$ is not equal to ${\nu }_{ji}$ : they are related by ${\nu }_{ij}/E_i$ = ${\nu }_{ji}/E_j$ . The engineering constants can also be given as functions of temperature and other predefined fields, if necessary.

In Abaqus/Standard spatially varying orthotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (Distribution Definition). The distribution must include default values for the elastic moduli and Poisson's ratios. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

A special subclass of orthotropy is transverse isotropy, which is characterized by a plane of isotropy at every point in the material. Assuming the 1–2 plane to be the plane of isotropy at every point, transverse isotropy requires that $E_1$ = $E_2$ = $E_p$ , ${\nu }_{31}$ = ${\nu }_{32}$ = ${\nu }_{tp}$ , ${\nu }_{13}$ = ${\nu }_{23}$ = ${\nu }_{pt}$ , and $G_{13}$ = $G_{23}$ = $G_t$ , where p and t stand for “in-plane” and “transverse,” respectively. Thus, while ${\nu }_{tp}$ has the physical interpretation of the Poisson's ratio that characterizes the strain in the plane of isotropy resulting from stress normal to it, ${\nu }_{pt}$ characterizes the transverse strain in the direction normal to the plane of isotropy resulting from stress in the plane of isotropy. In general, the quantities ${\nu }_{tp}$ and ${\nu }_{pt}$ are not equal and are related by ${\nu }_{tp}/E_t$ = ${\nu }_{pt}/E_p$ . The stress-strain laws reduce to

where $G_p$ = $E_p/2\left(1+{\nu }_p\right)$ and the total number of independent constants is only five.

In Abaqus/Standard spatially varying transverse isotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (Distribution Definition). The distribution must include default values for the elastic moduli and Poisson's ratio. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

Under plane stress conditions, such as in a shell element, only the values of $E_1$ , $E_2$ , ${\nu }_{12}$ , $G_{12}$ , $G_{13}$ , and $G_{23}$ are required to define an orthotropic material. (In all of the plane stress elements in Abaqus the $\left(1,2\right)$ surface is the surface of plane stress, so that the plane stress condition is ${\sigma }_{33}=0$ .) The shear moduli $G_{13}$ and $G_{23}$ are included because they might be required for modeling transverse shear deformation in a shell. The Poisson's ratio ${\nu }_{21}$ is implicitly given as ${\nu }_{21}=\left(E_2/E_1\right){\nu }_{12}$ . In this case the stress-strain relations for the in-plane components of the stress and strain are of the form

In Abaqus/Standard spatially varying plane stress orthotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (Distribution Definition). The distribution must include default values for the elastic moduli and Poisson's ratio. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

Under plane stress conditions, Abaqus/Explicit allows you to define different orthotropic elastic properties in tension and compression. This type of elasticity definition is called bilamina elasticity. The stress-strain relations for the in-plane components of the stress and strain are of the form

where the values of the elastic constants $E_1$ , $E_2$ , and ${\nu }_{12}$ are interpolated between their tensile values ( $E_{1+}$ , $E_{2+}$ , and ${\nu }_{12+}$ ) and compressive values ( $E_{1-}$ , $E_{2-}$ , and ${\nu }_{12-}$ ) based on a criterion depending on the invariants of the strain tensor.

Linear elasticity in an orthotropic material can also be defined by giving the nine independent elastic stiffness parameters, as functions of temperature and other predefined fields, if necessary. In this case the stress-strain relations are of the form

For an orthotropic material the engineering constants define the $\mathbf{D}$ matrix as

where

When the material stiffness parameters (the $D_{ijkl}$ ) are given directly, Abaqus imposes the constraint ${\sigma }_{33}=0$ for the plane stress case to reduce the material's stiffness matrix as required.

In Abaqus/Standard spatially varying orthotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (Distribution Definition). The distribution must include default values for the elastic moduli. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

For fully anisotropic elasticity 21 independent elastic stiffness parameters are needed. The stress-strain relations are as follows:

When the material stiffness parameters (the $D_{ijkl}$ ) are given directly, Abaqus imposes the constraint ${\sigma }_{33}=0$ for the plane stress case to reduce the material's stiffness matrix as required.

In Abaqus/Standard spatially varying anisotropic elastic behavior can be defined for homogeneous solid continuum elements by using a distribution (Distribution Definition). The distribution must include default values for the elastic moduli. If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

For two-dimensional meshed models of solid cross-section Timoshenko beam elements modeled with 1-DOF warping elements (see Meshed Beam Cross-Sections), Abaqus offers a linear elastic material definition that can have two different shear moduli in the user-specified material directions. In the user-specified directions the stress-strain relations are as follows:

A local orientation is used to define the angle $\alpha$ between the global directions and the user-specified material directions. In the cross-section directions the stress-strain relations are as follows:

where $\sigma$ represents the beam's axial stress and ${\tau }_1$ and ${\tau }_2$ represent two shear stresses.

For cohesive elements used to model bonded interfaces (see Defining the Constitutive Response of Cohesive Elements Using a Traction-Separation Description) Abaqus offers an elasticity definition that can be written directly in terms of the nominal tractions and the nominal strains. Both uncoupled and coupled behaviors are supported. For uncoupled behavior each traction component depends only on its conjugate nominal strain, while for coupled behavior the response is more general (as shown below). In the local element directions the stress-strain relations for uncoupled behavior are as follows:

The quantities $t_n$ , $t_s$ , and $t_t$ represent the nominal tractions in the normal and the two local shear directions, respectively; while the quantities ${\epsilon }_n$ , ${\epsilon }_s$ , and ${\epsilon }_t$ represent the corresponding nominal strains. For coupled traction separation behavior the stress-strain relations are as follows:

Abaqus/Explicit allows you to define isotropic shear elasticity to describe the deviatoric response of materials whose volumetric response is governed by an equation of state (Elastic Shear Behavior). In this case the deviatoric stress-strain relationship is given by

where $\mathbf{S}$ is the deviatoric stress and ${\mathbf{e}}^{el}$ is the deviatoric elastic strain. You must provide the elastic shear modulus, $\mu$ , when you define the elastic deviatoric behavior.

Abaqus allows you to specify the initial elastic transverse shear moduli for computing the transverse shear stiffness of shells and beams. You can define isotropic, orthotropic, and anisotropic transverse shear moduli.

For beam elements, the material transverse shear stress-relations are as follows:

• Isotropic:

• Orthotropic:

• Anisotropic:

For shell elements, the material transverse shear stress-strain relations are as follows:

• Isotropic:

• Orthotropic:

• Anisotropic:

You can define the transverse shear moduli for materials for which estimates of the shear moduli are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by user subroutines UMAT, UHYPEL, UHYPER, or VUMAT. You can also define the transverse shear moduli to override the default values computed by a material behavior; for example, you can define anisotropic transverse shear moduli for an isotropic elastic material.

The transverse shear moduli that you define are used only to compute the transverse shear stiffness at the beginning of the analysis. Any change to the transverse shear moduli during the analysis is ignored. The transverse shear moduli of a material are ignored if nondefault values of the transverse shear stiffness are specified for a section that is associated with the material (see Defining the Transverse Shear Stiffness for shell sections, Defining the Transverse Shear Stiffness for general shell sections, and Transverse Shear Stiffness Definition for beams).

You can define the elasticity of a short-fiber reinforced composite (for example, an injection molded composite) by specifying an orientation tensor (see Specifying a Second-Order Orientation Tensor in Abaqus/Standard and Specifying a Second-Order Orientation Tensor in Abaqus/Explicit) and the elastic modulus of a unidirectional (UD) composite. If the elasticity of the unidirectional composite is transversely isotropic (see Defining Transversely Isotropic Elasticity), the elasticity can then be computed using orientation averaging (Advani and Tucker, 1987):

where $D_1$ , $D_2$ , $D_3$ , $D_4$ , and $D_5$ are the five constants of the stiffness matrix of the unidirectional composite (the 1-direction is the fiber direction of the unidirectional composite):

$a_{ij}$ is the second-order orientation tensor; and ${\delta }_{ij}$ is the Kronecker delta. The fourth-order tensor $a_{ijkl}$ is computed using the second-order orientation tensor with closure approximations (Cintra and Tucker, 1995). Abaqus uses the closure approximations that result in an orthotropic stiffness with the principal directions aligned with those of the second-order orientation tensor. Since the elasticity is orthotropic, you must define the material directions with local orientations (see Orientations), and the axes of the local system must align with the principal directions of the second-order orientation tensor.