# Elements The plane stress orthotropic failure measures can be used with any plane stress, shell, or membrane element in Abaqus. # Output Abaqus provides output of the failure index, R, if failure measures are defined with the material description. The definition of the failure index and the different output variables are described below. # Output failure indices Each of the stress-based failure theories defines a failure surface surrounding the origin in the threedimensional space $\left\{ \sigma _ { 1 1 } , \sigma _ { 2 2 } , \sigma _ { 1 2 } \right\}$ . Failure occurs any time a state of stress is either on or outside this surface. The failure index, R, is used to measure the proximity to the failure surface. R is defined as the scaling factor such that, for the given stress state $\left\{ \sigma _ { 1 1 } , \sigma _ { 2 2 } , \sigma _ { 1 2 } \right\}$ , $$ \left\{\frac {\sigma_ {1 1}}{R}, \frac {\sigma_ {2 2}}{R}, \frac {\sigma_ {1 2}}{R} \right\} \Rightarrow I _ {F} = 1. 0; $$ that is, $1 / R$ is the scaling factor with which we need to multiply all of the stress components simultaneously to lie on the failure surface. Values $R < 1 . 0$ indicate that the state of stress is within the failure surface, while values $R \geq 1 . 0$ indicate failure. For the maximum stress theory $R \equiv I _ { F }$ . The failure index R is defined similarly for the maximum strain failure theory. R is the scaling factor such that, for the given strain state $\left\{ \varepsilon _ { 1 1 } , \varepsilon _ { 2 2 } , \varepsilon _ { 1 2 } \right\}$ , $$ \left\{\frac {\varepsilon_ {1 1}}{R}, \frac {\varepsilon_ {2 2}}{R}, \frac {\varepsilon_ {1 2}}{R} \right\} \Rightarrow I _ {F} = 1. 0. $$ For the maximum strain theory $R \equiv I _ { F }$ . # Output variables Output variable CFAILURE will provide output for all of the stress- and strain-based failure theories (see “Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2). In Abaqus/Standard history output can also be requested for the individual stress theories with output variables MSTRS, TSAIH, TSAIW, and AZZIT and for the strain theory with output variable MSTRN. Output variables for the stress- and strain-based failure theories are always calculated at the material points of the element. In Abaqus/Standard element output can be requested at a location other than the material points (see “Output to the data and results files,” Section 4.1.2); in this case the output variables are first calculated at the material points, then interpolated to the element centroid or extrapolated to the nodes. # 22.3 Porous elasticity • “Elastic behavior of porous materials,” Section 22.3.1 # 22.3.1 ELASTIC BEHAVIOR OF POROUS MATERIALS Products: Abaqus/Standard Abaqus/CAE # References • “Material library: overview,” Section 21.1.1 • “Elastic behavior: overview,” Section 22.1.1 • \*POROUS ELASTIC • \*INITIAL CONDITIONS • “Creating a porous elastic material model” in “Defining elasticity,” Section 12.9.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide # Overview A porous elastic material model: • is valid for small elastic strains (normally less than 5%); • is a nonlinear, isotropic elasticity model in which the pressure stress varies as an exponential function of volumetric strain; • allows a zero or nonzero elastic tensile stress limit; and • can have properties that depend on temperature and other field variables. # Defining the volumetric behavior Often, the elastic part of the volumetric behavior of porous materials is modeled accurately by assuming that the elastic part of the change in volume of the material is proportional to the logarithm of the pressure stress (Figure 22.3.1–1): $$ \frac {\kappa}{(1 + e _ {0})} \ln \left(\frac {p _ {0} + p _ {t} ^ {e l}}{p + p _ {t} ^ {e l}}\right) = J ^ {e l} - 1, $$ where is the “logarithmic bulk modulus”; $e _ { 0 }$ is the initial void ratio; p is the equivalent pressure stress, defined by $$ p = - \frac {1}{3} \operatorname{trace} \boldsymbol {\sigma} = - \frac {1}{3} \left(\sigma_ {1 1} + \sigma_ {2 2} + \sigma_ {3 3}\right); $$ $p _ { 0 }$ is the initial value of the equivalent pressure stress; $J ^ { e l }$ is the elastic part of the volume ratio between the current and reference configurations; and $p _ { t } ^ { e l }$ is the “elastic tensile strength” of the material (in the sense that $J ^ { e l } \to \infty \mathrm { a s } p \to - p _ { t } ^ { e l } )$ . Input File Usage: Use all three of the following options to define a porous elastic material: \*POROUS ELASTIC, SHEAR=G or POISSON to define and $p _ { t } ^ { e l }$ 

line

| ε^el_vol | p | | -------- | ------- | | - | -p_t^el | | p_0 | p_0 | | p_t^el | -p_t^el |

Figure 22.3.1–1 Porous elastic volumetric behavior. \*INITIAL CONDITIONS, TYPE=STRESS to define $p _ { 0 }$ \*INITIAL CONDITIONS, TYPE=RATIO to define $e _ { 0 }$ Abaqus/CAE Usage: Use all three of the following options to define a porous elastic material: Property module: material editor: Mechanical→Elasticity→Porous Elastic Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress for the Types for Selected Step Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step # Defining the shear behavior The deviatoric elastic behavior of a porous material can be defined in either of two ways. # By defining the shear modulus Give the shear modulus, G. The deviatoric stress, , is then related to the deviatoric part of the total elastic strain, $\mathbf { e } ^ { e l }$ , by $$ \mathbf {S} = 2 G \mathbf {e} ^ {e l}. $$ In this case the shear behavior is not affected by compaction of the material. Input File Usage: \*POROUS ELASTIC, SHEAR=G # Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Porous Elastic: Shear: G # By defining Poisson’s ratio Define Poisson’s ratio, . The instantaneous shear modulus is then defined from the instantaneous bulk modulus and Poisson’s ratio as $$ G = \frac {3 (1 - 2 \nu) (1 + e _ {0})}{2 (1 + \nu) \kappa} (p + p _ {t} ^ {e l}) \exp (\varepsilon_ {v o l} ^ {e l}), $$ where $\varepsilon _ { v o l } ^ { e l } = \ln J ^ { e l }$ is the logarithmic measure of the elastic volume change. In this case $$ d \mathbf {S} = 2 G d \mathbf {e} ^ {e l}. $$ Thus, the elastic shear stiffness increases as the material is compacted. This equation is integrated to give the total stress–total elastic strain relationship. Input File Usage: \*POROUS ELASTIC, SHEAR=POISSON Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Porous Elastic: Shear: Poisson # Use with other material models The porous elasticity model can be used by itself, or it can be combined with: • the “Extended Drucker-Prager models,” Section 23.3.1; • the “Modified Drucker-Prager/Cap model,” Section 23.3.2; • the “Critical state (clay) plasticity model,” Section 23.3.4; or • isotropic expansion to introduce thermal volume changes (“Thermal expansion,” Section 26.1.2). It is not possible to use porous elasticity with rate-dependent plasticity or viscoelasticity. Porous elasticity cannot be used with the porous metal plasticity model (“Porous metal plasticity,” Section 23.2.9). See “Combining material behaviors,” Section 21.1.3, for more details. # Elements Porous elasticity cannot be used with hybrid elements or plane stress elements (including shells and membranes), but it can be used with any other pure stress/displacement element in Abaqus/Standard. If used with reduced-integration elements with total-stiffness hourglass control, Abaqus/Standard cannot calculate a default value for the hourglass stiffness of the element if the shear behavior is defined through Poisson’s ratio. Hence, you must specify the hourglass stiffness. See “Section controls,” Section 27.1.4, for details. If fluid pore pressure is important (such as in undrained soils), stress/displacement elements that include pore pressure can be used. # 22.4 Hypoelasticity • “Hypoelastic behavior,” Section 22.4.1