Linear Elastic Behavior

Defining Linear Elastic Material Behavior

The total stress is defined from the total elastic strain as

σ = D^{e l} ε^{e l},

where $σ$ is the total stress (“true,” or Cauchy stress in finite-strain problems), $D^{e l}$ is the fourth-order elasticity tensor, and $ε^{e l}$ 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%).

Defining Linear Elastic Response for Viscoelastic Materials

The elastic response of a viscoelastic material (Time Domain Viscoelasticity) can be specified by defining either the instantaneous response or the long-term response of the material.

Instantaneous Response

To define the instantaneous response, experiments to determine the elastic constants must be performed within time spans much shorter than the characteristic relaxation time of the material.

Input File Usage

ELASTIC, MODULI=INSTANTANEOUS

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Moduli time scale (for viscoelasticity): Instantaneous

Long-Term Response

However, if the long-term elastic response is used, data from experiments must be collected after time spans much longer than the characteristic relaxation time of the viscoelastic material. Long-term elastic response is the default elastic material behavior.

Input File Usage

ELASTIC, MODULI=LONG TERM

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Moduli time scale (for viscoelasticity): Long-term

Directional Dependence of Linear Elasticity

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 $D^{e l}$ 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.

Stability of a Linear Elastic Material

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 $D^{e l}$ 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.

Defining Isotropic Elasticity

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

{\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} = [\begin{matrix} 1 / E & - ν / E & - ν / E & 0 & 0 & 0 \\ - ν / E & 1 / E & - ν / E & 0 & 0 & 0 \\ - ν / E & - ν / E & 1 / E & 0 & 0 & 0 \\ 0 & 0 & 0 & 1 / G & 0 & 0 \\ 0 & 0 & 0 & 0 & 1 / G & 0 \\ 0 & 0 & 0 & 0 & 0 & 1 / G \end{matrix}] {\begin{matrix} σ_{11} \\ σ_{22} \\ σ_{33} \\ σ_{12} \\ σ_{13} \\ σ_{23} \end{matrix}} .

The elastic properties are completely defined by giving the Young's modulus, E, and the Poisson's ratio, $ν$ . The shear modulus, G, can be expressed in terms of E and $ν$ as $G = E / 2 (1 + ν)$ . 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 $ν$ . If a distribution is used, no dependencies on temperature and/or field variables for the elastic constants can be defined.

Input File Usage

ELASTIC, TYPE=ISOTROPIC

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Isotropic

Stability

The stability criterion requires that $E > 0$ , $G > 0$ , and $- 1 < ν < 0.5$ . Values of Poisson's ratio approaching 0.5 result in nearly incompressible behavior. With the exception of plane stress cases (including membranes and shells) or beams and trusses, such values require the use of “hybrid” elements in Abaqus/Standard and generate high frequency noise and result in excessively small stable time increments in Abaqus/Explicit.

In Abaqus/Standard it is recommended that you use solid continuum hybrid elements for linear elastic materials with Poisson's ratio greater than 0.495 (that is, the ratio of $K / μ$ greater than 100) to avoid potential convergence problems. Otherwise, the analysis preprocessor will issue an error. You can use the “nonhybrid incompressible” diagnostics control to downgrade this error to a warning message.

Input File Usage

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

DIAGNOSTICS, NONHYBRID INCOMPRESSIBLE=WARNING

Defining Orthotropic Elasticity by Specifying the Engineering Constants

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 $ν_{12}$ , $ν_{13}$ , $ν_{23}$ ; 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

{\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} = [\begin{matrix} 1 / E_{1} & - ν_{21} / E_{2} & - ν_{31} / E_{3} & 0 & 0 & 0 \\ - ν_{12} / E_{1} & 1 / E_{2} & - ν_{32} / E_{3} & 0 & 0 & 0 \\ - ν_{13} / E_{1} & - ν_{23} / E_{2} & 1 / E_{3} & 0 & 0 & 0 \\ 0 & 0 & 0 & 1 / G_{12} & 0 & 0 \\ 0 & 0 & 0 & 0 & 1 / G_{13} & 0 \\ 0 & 0 & 0 & 0 & 0 & 1 / G_{23} \end{matrix}] {\begin{matrix} σ_{11} \\ σ_{22} \\ σ_{33} \\ σ_{12} \\ σ_{13} \\ σ_{23} \end{matrix}} .

The quantity $ν_{i j}$ 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, $ν_{i j}$ is not equal to $ν_{j i}$ : they are related by $ν_{i j} / E_{i}$ = $ν_{j i} / E_{j}$ . 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.

Input File Usage

ELASTIC, TYPE=ENGINEERING CONSTANTS

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Engineering Constants

Stability

Material stability requires

\begin{matrix} E_{1}, E_{2}, E_{3}, G_{12}, G_{13}, G_{23} > 0, \\ | ν_{12} | < {(E_{1} / E_{2})}^{1 / 2}, \\ | ν_{13} | < {(E_{1} / E_{3})}^{1 / 2}, \\ | ν_{23} | < {(E_{2} / E_{3})}^{1 / 2}, \\ 1 - ν_{12} ν_{21} - ν_{23} ν_{32} - ν_{31} ν_{13} - 2 ν_{21} ν_{32} ν_{13} > 0. \end{matrix}

When the left-hand side of the inequality approaches zero, the material exhibits incompressible behavior. Using the relations $ν_{i j} / E_{i}$ = $ν_{j i} / E_{j}$ , the second, third, and fourth restrictions in the above set can also be expressed as

\begin{matrix} | ν_{21} | < {(E_{2} / E_{1})}^{1 / 2}, \\ | ν_{31} | < {(E_{3} / E_{1})}^{1 / 2}, \\ | ν_{32} | < {(E_{3} / E_{2})}^{1 / 2} . \end{matrix}

Defining Transversely Isotropic Elasticity

A special subclass of orthotropy is transverse isotropy, which is characterized by a plane of isotropy at every point in the material. Abaqus assumes the 2-3 plane to be the plane of isotropy at every point; therefore, transverse isotropy requires that $E_{2}$ = $E_{3}$ , $ν_{12}$ = $ν_{13}$ , $ν_{21}$ = $ν_{31}$ , $ν_{23}$ = $ν_{32}$ , and $G_{12}$ = $G_{13}$ , and $G_{23}$ = $E_{2} / 2 (1 + ν_{23})$ . The stress-strain laws reduce to

{\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} = [\begin{matrix} 1 / E_{1} & - ν_{21} / E_{2} & - ν_{21} / E_{2} & 0 & 0 & 0 \\ - ν_{12} / E_{1} & 1 / E_{2} & - ν_{32} / E_{2} & 0 & 0 & 0 \\ - ν_{12} / E_{1} & - ν_{23} / E_{2} & 1 / E_{2} & 0 & 0 & 0 \\ 0 & 0 & 0 & 1 / G_{12} & 0 & 0 \\ 0 & 0 & 0 & 0 & 1 / G_{12} & 0 \\ 0 & 0 & 0 & 0 & 0 & 1 / G_{23} \end{matrix}] {\begin{matrix} σ_{11} \\ σ_{22} \\ σ_{33} \\ σ_{12} \\ σ_{13} \\ σ_{23} \end{matrix}},

where the total number of independent constants is only five.

Input File Usage

ELASTIC, TYPE=TRANSVERSELY ISOTROPIC

Abaqus/CAE Usage

Specifying the elasticity of a transversely isotropic material is not supported in Abaqus/CAE.

Stability

In the transversely isotropic case the stability relations for orthotropic elasticity simplify to

\begin{matrix} E_{1}, E_{2}, G_{12}, G_{23} > 0, \\ | ν_{12} | < {(E_{1} / E_{2})}^{1 / 2}, \\ | ν_{21} | < {(E_{2} / E_{1})}^{1 / 2}, \\ | ν_{23} | < 1.0, \\ 1 - ν_{23}^{2} - 2 ν_{12} ν_{21} - 2 ν_{21} ν_{32} ν_{12} > 0. \end{matrix}

Defining Orthotropic Elasticity in Plane Stress

Under plane stress conditions, such as in a shell element, only the values of $E_{1}$ , $E_{2}$ , $ν_{12}$ , $G_{12}$ , $G_{13}$ , and $G_{23}$ are required to define an orthotropic material. (In all of the plane stress elements in Abaqus the $(1, 2)$ surface is the surface of plane stress, so that the plane stress condition is $σ_{33} = 0$ .) 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 $ν_{21}$ is implicitly given as $ν_{21} = (E_{2} / E_{1}) ν_{12}$ . In this case the stress-strain relations for the in-plane components of the stress and strain are of the form

{\begin{matrix} ε_{1} \\ ε_{2} \\ γ_{12} \end{matrix}} = [\begin{matrix} 1 / E_{1} & - ν_{12} / E_{1} & 0 \\ - ν_{12} / E_{1} & 1 / E_{2} & 0 \\ 0 & 0 & 1 / G_{12} \end{matrix}] {\begin{matrix} σ_{11} \\ σ_{22} \\ τ_{12} \end{matrix}} .

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.

Input File Usage

ELASTIC, TYPE=LAMINA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Lamina

Stability

Material stability for plane stress requires

\begin{matrix} E_{1}, E_{2}, G_{12}, G_{13}, G_{23} > 0, \\ | ν_{12} | < {(E_{1} / E_{2})}^{1 / 2} . \end{matrix}

Defining Orthotropic Elasticity in Plane Stress with Different Moduli in Tension and Compression

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

{\begin{matrix} ε_{1} \\ ε_{2} \\ γ_{12} \end{matrix}} = [\begin{matrix} 1 / E_{1} & - ν_{12} / E_{1} & 0 \\ - ν_{12} / E_{1} & 1 / E_{2} & 0 \\ 0 & 0 & 1 / G_{12} \end{matrix}] {\begin{matrix} σ_{11} \\ σ_{22} \\ τ_{12} \end{matrix}},

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

Input File Usage

ELASTIC, TYPE=BILAMINA

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Bilamina

Stability

Material stability for plane stress requires

\begin{matrix} E_{1 +}, E_{2 +}, G_{12}, E_{1 -}, E_{2 -} > 0, \\ | ν_{12 +} | < {(E_{1 +} / E_{2 +})}^{1 / 2}, \\ | ν_{12 -} | < {(E_{1 -} / E_{2 -})}^{1 / 2} . \end{matrix}

Defining Orthotropic Elasticity by Specifying the Terms in the Elastic Stiffness Matrix

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

{\begin{matrix} σ_{11} \\ σ_{22} \\ σ_{33} \\ σ_{12} \\ σ_{13} \\ σ_{23} \end{matrix}} = [\begin{matrix} D_{1111} & D_{1122} & D_{1133} & 0 & 0 & 0 \\ D_{2222} & D_{2233} & 0 & 0 & 0 \\ D_{3333} & 0 & 0 & 0 \\ D_{1212} & 0 & 0 \\ s y m & D_{1313} & 0 \\ D_{2323} \end{matrix}] {\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} = [D^{e l}] {\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} .

For an orthotropic material the engineering constants define the $D$ matrix as

\begin{matrix} D_{1111} = E_{1} (1 - ν_{23} ν_{32}) Υ, \\ D_{2222} = E_{2} (1 - ν_{13} ν_{31}) Υ, \\ D_{3333} = E_{3} (1 - ν_{12} ν_{21}) Υ, \\ D_{1122} = E_{1} (ν_{21} + ν_{31} ν_{23}) Υ = E_{2} (ν_{12} + ν_{32} ν_{13}) Υ, \\ D_{1133} = E_{1} (ν_{31} + ν_{21} ν_{32}) Υ = E_{3} (ν_{13} + ν_{12} ν_{23}) Υ, \\ D_{2233} = E_{2} (ν_{32} + ν_{12} ν_{31}) Υ = E_{3} (ν_{23} + ν_{21} ν_{13}) Υ, \\ D_{1212} = G_{12}, \\ D_{1313} = G_{13}, \\ D_{2323} = G_{23}, \end{matrix}

where

Υ = \frac{1}{1 - ν_{12} ν_{21} - ν_{23} ν_{32} - ν_{31} ν_{13} - 2 ν_{21} ν_{32} ν_{13}} .

When the material stiffness parameters (the $D_{i j k l}$ ) are given directly, Abaqus imposes the constraint $σ_{33} = 0$ 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.

Input File Usage

ELASTIC, TYPE=ORTHOTROPIC

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Orthotropic

Stability

The restrictions on the elastic constants due to material stability are

\begin{matrix} D_{1111}, D_{2222}, D_{3333}, D_{1212}, D_{1313}, D_{2323} > 0, \\ | D_{1122} | < {(D_{1111} D_{2222})}^{1 / 2}, \\ | D_{1133} | < {(D_{1111} D_{3333})}^{1 / 2}, \\ | D_{2233} | < {(D_{2222} D_{3333})}^{1 / 2}, \\ d e t (D^{e l}) > 0. \end{matrix}

The last relation leads to

D_{1111} D_{2222} D_{3333} + 2 D_{1122} D_{1133} D_{2233} - D_{2222} D_{1133}^{2} - D_{1111} D_{2233}^{2} - D_{3333} D_{1122}^{2} > 0.

These restrictions in terms of the elastic stiffness parameters are equivalent to the restrictions in terms of the “engineering constants.” Incompressible behavior results when the left-hand side of the inequality approaches zero.

Defining Fully Anisotropic Elasticity

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

{\begin{matrix} σ_{11} \\ σ_{22} \\ σ_{33} \\ σ_{12} \\ σ_{13} \\ σ_{23} \end{matrix}} = [\begin{matrix} D_{1111} & D_{1122} & D_{1133} & D_{1112} & D_{1113} & D_{1123} \\ D_{2222} & D_{2233} & D_{2212} & D_{2213} & D_{2223} \\ D_{3333} & D_{3312} & D_{3313} & D_{3323} \\ D_{1212} & D_{1213} & D_{1223} \\ s y m & D_{1313} & D_{1323} \\ D_{2323} \end{matrix}] {\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} = [D^{e l}] {\begin{matrix} ε_{11} \\ ε_{22} \\ ε_{33} \\ γ_{12} \\ γ_{13} \\ γ_{23} \end{matrix}} .

When the material stiffness parameters (the $D_{i j k l}$ ) are given directly, Abaqus imposes the constraint $σ_{33} = 0$ 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.

Input File Usage

ELASTIC, TYPE=ANISOTROPIC

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Anisotropic

Stability

The restrictions imposed on the elastic constants by stability requirements are too complex to express in terms of simple equations. However, the requirement that $D^{e l}$ is positive definite requires that all of the eigenvalues of the elasticity matrix $[D^{e l}]$ be positive.

Defining Orthotropic Elasticity for 1-DOF Warping Elements

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:

{\begin{matrix} σ \\ τ_{1} \\ τ_{2} \end{matrix}} = [\begin{matrix} E \\ G_{1} \\ G_{2} \end{matrix}] {\begin{matrix} ε \\ γ_{1} \\ γ_{2} \end{matrix}} .

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

{\begin{matrix} σ \\ τ_{1} \\ τ_{2} \end{matrix}} = [\begin{matrix} E & 0 & 0 \\ G_{1} {(\cos α)}^{2} + G_{2} {(\sin α)}^{2} & (G_{1} - G_{2}) \cos α \sin α \\ s y m & G_{1} {(\sin α)}^{2} + G_{2} {(\cos α)}^{2} \end{matrix}] {\begin{matrix} ε \\ γ_{1} \\ γ_{2} \end{matrix}},

where $σ$ represents the beam's axial stress and $τ_{1}$ and $τ_{2}$ represent two shear stresses.

Input File Usage

ELASTIC, TYPE=TRACTION

Abaqus/CAE Usage

Property module: material editor: MechanicalElasticityElastic: Type: Traction

Stability

The stability criterion requires that $E > 0$ , $G_{1} > 0$ , and $G_{2} > 0$ .

Defining Elasticity in Terms of Tractions and Separations for Cohesive Elements

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:

{\begin{matrix} t_{n} \\ t_{s} \\ t_{t} \end{matrix}} = [\begin{matrix} E_{n n} \\ E_{s s} \\ E_{t t} \end{matrix}] {\begin{matrix} ε_{n} \\ ε_{s} \\ ε_{t} \end{matrix}} .

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 $ε_{n}$ , $ε_{s}$ , and $ε_{t}$ represent the corresponding nominal strains. For coupled traction separation behavior the stress-strain relations are as follows:

{\begin{matrix} t_{n} \\ t_{s} \\ t_{t} \end{matrix}} = [\begin{matrix} E_{n n} & E_{n s} & E_{n t} \\ E_{n s} & E_{s s} & E_{s t} \\ E_{n t} & E_{s t} & E_{t t} \end{matrix}] {\begin{matrix} ε_{n} \\ ε_{s} \\ ε_{t} \end{matrix}} .

Input File Usage

Use the following option to define uncoupled elastic behavior for cohesive elements:

ELASTIC, TYPE=TRACTION

Use the following option to define coupled elastic behavior for cohesive elements:

ELASTIC, TYPE=COUPLED TRACTION

Abaqus/CAE Usage

Use the following option to define uncoupled elastic behavior for cohesive elements:

Property module: material editor: MechanicalElasticityElastic: Type: Traction

Use the following option to define coupled elastic behavior for cohesive elements:

Property module: material editor: MechanicalElasticityElastic: Type: Coupled Traction

Stability

The stability criterion for uncoupled behavior requires that $E_{n n} > 0$ , $E_{s s} > 0$ , and $E_{t t} > 0$ . For coupled behavior the stability criterion requires that:

E_{n n} > 0, E_{s s} > 0, E_{t t} > 0;

E_{n s} < \sqrt{E_{n n} E_{s s}};

E_{s t} < \sqrt{E_{s s} E_{t t}};

E_{n t} < \sqrt{E_{n n} E_{t t}};

d e t [\begin{matrix} E_{n n} & E_{n s} & E_{n t} \\ E_{n s} & E_{s s} & E_{s t} \\ E_{n t} & E_{s t} & E_{t t} \end{matrix}] > 0.

Cohesive Offset

A cohesive offset (Figure 1) refers to a value of the separation in the normal direction, $δ_{n} = δ_{n}^{o f f}$ , below which the resistance to additional closure $(δ_{n} > 0, {\dot{δ}}_{n} < 0)$ of the cohesive surfaces increases significantly. This capability is useful in preventing the closure of a fracture when changes in external loading conditions might otherwise result in closure. A practical application of this capability occurs during hydraulic fracturing with slurry, where solid proppant particles (the solid part of the slurry) help "prop open" the fracture when external hydraulic pressure loads are removed.

You can specify an offset to the separation in the normal direction for the following classes of cohesive elements:

pore pressure;
coupled temperature-pore pressure;
coupled slurry concentration-pore pressure; and
coupled temperature-slurry concentration-pore pressure.

You must specify the offset through user subroutine UCOHESIVEOFFSET. In addition to defining an offset, you can also define the stress or the Jacobian matrix for the traction-separation behavior.

If you do not define the stress in user subroutine UCOHESIVEOFFSET, Abaqus/Standard computes the normal component of the effective traction as $t_{n} = E_{n n} (ε_{n} - ε_{n}^{o f f})$ for an uncoupled traction-separation response and as $t_{n} = E_{n n} (ε_{n} - ε_{n}^{o f f}) + E_{n s} ε_{s} + E_{n t} ε_{t}$ for coupled traction behavior. In the expressions above for $t_{n}$ , $ε_{n}^{o f f} = \frac{δ_{n}^{o f f}}{T_{0}}$ , where $T_{0}$ is the original thickness of the cohesive element.

Subsequently, the effective traction is degraded due to progressive damage.

Input File Usage

Use the following option to define the cohesive offset for uncoupled elastic traction-separation behavior:

ELASTIC, TYPE=TRACTION, COHESIVE OFFSET=USER

Use the following option to define the cohesive offset for coupled elastic traction-separation behavior:

ELASTIC, TYPE=COUPLED TRACTION, COHESIVE OFFSET=USER

COHESIVE OFFSET=USER must be used in conjunction with either TYPE=COUPLED TRACTION or TYPE=TRACTION. And also a user subroutine UCOHESIVEOFFSET must be associated with this option.

Abaqus/CAE Usage

Specifying the cohesive offset is not supported in Abaqus/CAE.

Defining Isotropic Shear Elasticity for Equations of State in Abaqus/Explicit

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

S = 2 μ e^{e l},

where

S

is the deviatoric stress and

e^{e l}

is the deviatoric elastic strain. You must provide the elastic shear modulus,

μ

, when you define the elastic deviatoric behavior.

Input File Usage

ELASTIC, TYPE=SHEAR

Abaqus/CAE Usage

Property module: material editor: Mechanical Elasticity Elastic : Type: Shear

Defining the Elastic Transverse Shear Modulus

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:

{\begin{matrix} σ_{12} \\ σ_{13} \end{matrix}} = [\begin{matrix} G & 0 \\ 0 & G \end{matrix}] {\begin{matrix} γ_{12} \\ γ_{13} \end{matrix}}

Orthotropic:

{\begin{matrix} σ_{12} \\ σ_{13} \end{matrix}} = [\begin{matrix} G_{12} & 0 \\ 0 & G_{13} \end{matrix}] {\begin{matrix} γ_{12} \\ γ_{13} \end{matrix}}

Anisotropic:

{\begin{matrix} σ_{12} \\ σ_{13} \end{matrix}} = [\begin{matrix} D_{1212} & D_{1213} \\ D_{1213} & D_{1313} \end{matrix}] {\begin{matrix} γ_{12} \\ γ_{13} \end{matrix}}

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

Isotropic:

{\begin{matrix} σ_{13} \\ σ_{23} \end{matrix}} = [\begin{matrix} G & 0 \\ 0 & G \end{matrix}] {\begin{matrix} γ_{13} \\ γ_{23} \end{matrix}}

Orthotropic:

{\begin{matrix} σ_{13} \\ σ_{23} \end{matrix}} = [\begin{matrix} G_{13} & 0 \\ 0 & G_{23} \end{matrix}] {\begin{matrix} γ_{13} \\ γ_{23} \end{matrix}}

Anisotropic:

{\begin{matrix} σ_{13} \\ σ_{23} \end{matrix}} = [\begin{matrix} D_{1313} & D_{1323} \\ D_{1323} & D_{2323} \end{matrix}] {\begin{matrix} γ_{13} \\ γ_{23} \end{matrix}}

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).

Input File Usage

Use the following option to specify an isotropic transverse shear modulus:

TRANSVERSE SHEAR, TYPE=ISOTROPIC (default)

Use the following option to specify orthotropic transverse shear moduli:

TRANSVERSE SHEAR, TYPE=ORTHOTROPIC

Use the following option to specify anisotropic transverse shear moduli:

TRANSVERSE SHEAR, TYPE=ANISOTROPIC

Abaqus/CAE Usage

Specifying the elastic transverse shear modulus is not supported in Abaqus/CAE.

Defining the Elasticity of a Short-Fiber Reinforced Composite

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):

[D^{e l}] = D_{1} a_{i j k l} + D_{2} (a_{i j} δ_{k l} + a_{k l} δ_{i j}) + D_{3} (a_{i k} δ_{j l} + a_{i l} δ_{j k} + a_{j l} δ_{i k} + a_{j k} δ_{i l}) + D_{4} δ_{i j} δ_{k l} + D_{5} (δ_{i k} δ_{j l} + δ_{i l} δ_{j k}),

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):

D_{1} = D_{1111}^{U D} + D_{2222}^{U D} - 2 D_{1122}^{U D} - {4 D}_{1212}^{U D},

D_{2} = D_{1122}^{U D} - D_{2233}^{U D},

D_{3} = D_{1212}^{U D} + \frac{1}{2} (D_{2233}^{U D} - D_{2222}^{U D}),

D_{4} = D_{2233}^{U D},

D_{5} = \frac{1}{2} (D_{2222}^{U D} - D_{2233}^{U D});

a_{i j}

is the second-order orientation tensor; and

δ_{i j}

is the Kronecker delta. The fourth-order tensor

a_{i j k l}

is computed using the second-order orientation tensor with closure approximations (Cintra and Tucker, 1995). Predictions of linear elastic properties are sensitive to the choice of closure approximation. Although there are many closure formulations available in Abaqus, it is recommended to use the orthotropic fitted (ORF) closure (Cintra and Tucker, 1995) or orthotropic equaivalent of the natural (ORE) closure (VerWeyst, 1998) formulation when predicting mechanical properties.

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.

Input File Usage

Use one of the following options to specify the elastic stiffness of the transversely isotropic unidirectional composite:

ELASTIC, TYPE=ENGINEERING CONSTANTS
ELASTIC, TYPE=ORTHOTROPIC

Use the following option to specify the second-order orientation tensor in the orientation definition in Abaqus/Explicit:

ORIENTATION, DISPERSION

Use the following option to specify the second-order orientation tensor with the quadratic closure approximation:

FIBER DISPERSION, CLOSURE=QUADRATIC

Use the following option to specify the second-order orientation tensor with the hybrid closure approximation:

FIBER DISPERSION, CLOSURE=HYBRID

Use the following option to specify the second-order orientation tensor with the orthotropic fitted (ORF) closure approximation:

FIBER DISPERSION, CLOSURE=FITTED

Use the following option to specify the second-order orientation tensor with the orthotropic equaivalent of the natural (ORE) closure approximation:

FIBER DISPERSION, CLOSURE=ORE

Use the following option to specify the second-order orientation tensor with the orthotropic smooth (ORS) closure approximation:

FIBER DISPERSION, CLOSURE=SMOOTH

Abaqus/CAE Usage

Specifying the elasticity of a short-fiber reinforced composite is not supported in Abaqus/CAE.

Elements

Linear elasticity can be used with any stress/displacement element or coupled temperature-displacement element in Abaqus. The exceptions are traction elasticity, which can be used only with 1-DOF warping elements and cohesive elements; coupled traction elasticity, which can be used only with cohesive elements; shear elasticity, which can be used only with solid (continuum) elements except plane stress elements; and, in Abaqus/Explicit, anisotropic elasticity, which is not supported for truss, rebar, pipe, and beam elements.

If the material is (almost) incompressible (Poisson's ratio $ν > 0.49$ for isotropic elasticity), hybrid elements should be used in Abaqus/Standard. Compressible anisotropic elasticity should not be used with second-order hybrid continuum elements: inaccurate results and/or convergence problems might occur.

References

Advani, S., and C. Tucker, “The Use of Tensors to Describe and Predict Fiber Orientation in Short Fiber Composites,” Journal of Rheology, vol. 31 (8), pp. 751–784, 1987.
Cintra, J., and C. Tucker, “Orthotropic Closure Approximations for Flow-induced Fiber Orientation,” Journal of Rheology, vol. 39, pp. 1095–1122, 1995.
VerWeyst, B.E., “Numerical Predictions of Flow-Induced Fiber Orientation in 3-D Geometries,” Ph.D. thesis, University of Illinois at Urbana-Champaign, 1998.