$$ \Phi = \left(\frac {q}{\sigma_ {y}}\right) ^ {2} + 2 q _ {1} f ^ {*} \cosh \left(- q _ {2} \frac {3 p}{2 \sigma_ {y}}\right) - \left(1 + q _ {3} f ^ {* 2}\right) = 0, $$ where the function $f ^ { * } ( f )$ models the rapid loss of stress carrying capacity that accompanies void coalescence. This function is defined in terms of the void volume fraction: $$ f ^ {*} = \left\{ \begin{array}{l l} f & \text {if} f \leq f _ {c}, \\ f _ {c} + \frac {\bar {f} _ {F} - f _ {c}}{f _ {F} - f _ {c}} (f - f _ {c}) & \text {if} f _ {c} < f < f _ {F}, \\ \bar {f} _ {F} & \text {if} f \geq f _ {F}, \end{array} \right. $$ where $$ \bar {f} _ {F} = \frac {q _ {1} + \sqrt {q _ {1} ^ {2} - q _ {3}}}{q _ {3}}. $$ In the above relationship $f _ { c }$ is a critical value of the void volume fraction, and $f _ { F }$ is the value of void volume fraction at which there is a complete loss of stress carrying capacity in the material. The userspecified parameters $f _ { c }$ and $f _ { F }$ model the material failure when $f _ { c } < f < f _ { F }$ , due to mechanisms such as micro fracture and void coalescence. When $f \geq f _ { F }$ , total failure at the material point occurs. In Abaqus/Explicit an element is removed once all of its material points have failed. Input File Usage: Use the following option in conjunction with the \*POROUS METAL PLASTICITY option: \*POROUS FAILURE CRITERIA Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity: Suboptions→Porous Failure Criteria # Specifying the initial relative density You can specify the initial relative density of the porous material, $r _ { 0 }$ , at material points or at nodes. If you do not specify the initial relative density, Abaqus will assign it a value of 1.0. # At material points You can specify the initial relative density as part of the porous metal plasticity material definition. Input File Usage: \*POROUS METAL PLASTICITY, RELATIVE DENSIT $\mathrm { Y } { = } r _ { 0 }$ Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity: Relative density: $r _ { 0 }$ # At nodes Alternatively, you can specify the initial relative density at nodes as initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1); these values are interpolated to the material points. The initial conditions are applied only if the relative density is not specified as part of the porous metal plasticity material definition. When a discontinuity of the initial relative density field occurs at the element boundaries, separate nodes must be used to define the elements at these boundaries, with multi-point constraints applied to make the nodal displacements and rotations equivalent. Input File Usage: \*INITIAL CONDITIONS, TYPE=RELATIVE DENSITY Abaqus/CAE Usage: Initial relative density is not supported in Abaqus/CAE. # Flow rule and hardening The presence of pressure in the yield condition results in nondeviatoric plastic strains. Plastic flow is assumed to be normal to the yield surface: $$ \dot {\varepsilon} ^ {p l} = \dot {\lambda} \frac {\partial \Phi}{\partial \pmb {\sigma}}. $$ The hardening of the fully dense matrix material is described through $\sigma _ { y } = \sigma _ { y } ( \bar { \varepsilon } _ { m } ^ { p l } )$ . The evolution of the equivalent plastic strain in the matrix material is obtained from the following equivalent plastic work expression: $$ (1 - f) \sigma_ {y} \dot {\bar {\varepsilon}} _ {m} ^ {p l} = \pmb {\sigma}: \dot {\pmb {\varepsilon}} ^ {p l}. $$ The model is illustrated in Figure 23.2.9–1, where the yield surfaces for different levels of void volume fraction are shown in the p–q plane.  Figure 23.2.9–1 Schematic of the yield surface in the $_ { p - q }$ plane. Figure 23.2.9–2 compares the behavior of a porous material (whose initial yield stress is $\sigma _ { y _ { 0 } } )$ i n tension and compression against the behavior of the perfectly plastic matrix material. In compression the porous material “hardens” due to closing of the voids, and in tension it “softens” due to growth and nucleation of the voids. 

line

| ε | σ (f₀ = 0) | σ (tension) | | ------- | ---------- | ----------- | | -ε | -σ_y₀ | -σ_y₀ | | 0 | σ_y₀ | σ_y₀ | | ε | σ_y₀ | σ_y₀ |

Figure 23.2.9–2 Schematic of uniaxial behavior of a porous metal (perfectly plastic matrix material with initial volume fraction of voids $= f _ { 0 } )$ . # Void growth and nucleation The total change in void volume fraction is given as $$ \dot {f} = \dot {f} _ {\mathrm{gr}} + \dot {f} _ {\mathrm{nucl}}, $$ where ${ \dot { f } } _ { \mathrm { g r } }$ is change due to growth of existing voids and $\dot { f } _ { \mathrm { n u c l } }$ is change due to nucleation of new voids. Growth of the existing voids is based on the law of conservation of mass and is expressed in terms of the void volume fraction: $$ \dot {f} _ {\mathrm{gr}} = (1 - f) \dot {\varepsilon} ^ {p l}: \mathbf {I}. $$ The nucleation of voids is given by a strain-controlled relationship: $$ \dot {f} _ {\mathrm{nucl}} = A \dot {\bar {\varepsilon}} _ {m} ^ {p l}, $$ where $$ A = \frac {f _ {N}}{s _ {N} \sqrt {2 \pi}} \exp \left[ - \frac {1}{2} \left(\frac {\bar {\varepsilon} _ {m} ^ {p l} - \varepsilon_ {N}}{s _ {N}}\right) ^ {2} \right]. $$ The normal distribution of the nucleation strain has a mean value $\varepsilon _ { N }$ and standard deviation $s _ { N } , \ f _ { N }$ is the volume fraction of the nucleated voids, and voids are nucleated only in tension. The nucleation function $A / f _ { N }$ is assumed to have a normal distribution, as shown in Figure 23.2.9–3 for different values of the standard deviation $s _ { N }$ . 

line

| ε̅_m^pl | A/f_N (Material 1) | A/f_N (Material 2) | | ------- | ------------------ | ------------------ | | 0 | 0 | 0 | | ε_N | 1/s_N1√2π | 1/s_N2√2π | | >ε_N | 0 | 0 |

Figure 23.2.9–3 Nucleation function $A / f _ { N }$ . Figure 23.2.9–4 shows the extent of softening in a uniaxial tension test of a porous material for different values of $f _ { N }$ . 

line

| ε | σ (f_N1) | σ (f_N2) | | ------- | -------- | -------- | | Low | Low | Low | | Peak | High | Medium | | High | High | Low |

Figure 23.2.9–4 Softening (in uniaxial tension) as a function of $f _ { N }$ . The following ranges of values are reported in the literature for typical metals: $\varepsilon _ { N } = 0 . 1 \mathrm { t o } 0 . 3 , s _ { N } =$ 0.05 to 0.1, and $f _ { N } = 0 . 0 4$ (see “Necking of a round tensile bar,” Section 1.1.9 of the Abaqus Benchmarks Guide). You specify these parameters, which can be defined as tabular functions of temperature and predefined field variables. Abaqus will include void nucleation in a tensile field only when you include it in the material definition. In Abaqus/Standard the accuracy of the implicit integration of the void nucleation and growth equation is controlled by prescribing the maximum allowable time increment in the automatic time incrementation scheme. Input File Usage: \*VOID NUCLEATION Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Porous Metal Plasticity: Suboptions→Void Nucleation # Initial conditions When we need to study the behavior of a material that has already been subjected to some work hardening, Abaqus allows you to prescribe initial conditions directly for the equivalent plastic strain, $\bar { \varepsilon } ^ { p l }$ (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step # Defining initial hardening conditions in a user subroutine For more complicated cases, initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI. Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING, USER Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined # Elements The porous metal plasticity model can be used with any stress/displacement elements other than onedimensional elements (beam, pipe, and truss elements) or elements for which the assumed stress state is plane stress (plane stress, shell, and membrane elements). # Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning in the porous metal plasticity model:

PEEQ	Equivalent plastic strain, $\bar{\varepsilon}^{pl} = \bar{\varepsilon}^{pl}|_{0} + \int \frac{\sigma: d\varepsilon^{pl}}{(1 - f)\sigma_{y}}$ , where $\bar{\varepsilon}^{pl}|_{0}$ is the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”).
VVF	Void volume fraction.
VVFG	Void volume fraction due to void growth.
VVFN	Void volume fraction due to void nucleation.

# Additional references • Gurson, A. L., “Continuum Theory of Ductile Rupture by Void Nucleation and Growth: Part I—Yield Criteria and Flow Rules for Porous Ductile Materials,” Journal of Engineering Materials and Technology, vol. 99, pp. 2–15, 1977. • Tvergaard, V., “Influence of Voids on Shear Band Instabilities under Plane Strain Condition,” International Journal of Fracture Mechanics, vol. 17, pp. 389–407, 1981. # 23.2.10 CAST IRON PLASTICITY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE # References • “Material library: overview,” Section 21.1.1 • “Combining material behaviors,” Section 21.1.3 • “Inelastic behavior,” Section 23.1.1 • \*CAST IRON COMPRESSION HARDENING • \*CAST IRON PLASTICITY • \*CAST IRON TENSION HARDENING • “Defining cast iron plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide # Overview The cast iron plasticity model: • is intended for the constitutive modeling of gray cast iron; • provides elastic-plastic behavior with different yield strengths, flow, and hardening in tension and compression; • is based on a yield function that depends on the maximum principal stress under tensile loading conditions and pressure-independent (von Mises type) behavior under compressive loading conditions; • allows for simultaneous inelastic dilatation and inelastic shearing under tensile loading conditions; • allows only inelastic shearing under compressive loading conditions; • is intended for the simulation of material response only under essentially monotonic loading conditions; and • cannot be used to model rate dependence. # Elastic and plastic behavior The cast iron plasticity model describes the mechanical behavior of gray cast iron, a material with a microstructure consisting of a distribution of graphite flakes in a steel matrix. In tension the graphite flakes act as stress concentrators, resulting in yielding as a function of the maximum principal stress, followed by brittle behavior. In compression the graphite flakes do not have an appreciable effect on the macroscopic response, resulting in a ductile behavior similar to that of many steels. You specify the elastic part of the response separately; only linear isotropic elasticity can be used (see “Linear elastic behavior,” Section 22.2.1). The elastic stiffness is assumed to be the same under tension and compression. The cast iron plasticity model is used to provide the value of the plastic “Poisson’s ratio,” which is the absolute value of the ratio of the transverse to the longitudinal plastic strain under uniaxial tension. The plastic Poisson’s ratio can vary with the plastic deformation. However, the model in Abaqus assumes that it is constant with respect to plastic deformation. It can depend on temperature and field variables. If no value is specified for the plastic Poisson’s ratio, a default value of 0.04 is assumed. This default value is based on experimental results for permanent volumetric strain under uniaxial tension (see “Cast iron plasticity,” Section 4.3.7 of the Abaqus Theory Guide, for details). Independent hardening (see Figure 23.2.10–1) of the material under tension and compression can be specified as described below. The tension hardening data provide the uniaxial tension yield stress as a function of plastic strain, temperature, and field variables under uniaxial tension. The compression hardening data provide the uniaxial compression yield stress as a function of plastic strain, temperature, and field variables under uniaxial compression. 

text_image

σ ε compression tension

Figure 23.2.10–1 Typical stress-strain response of gray cast iron under uniaxial tension and uniaxial compression. Input File Usage: \*CAST IRON PLASTICITY Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Cast Iron Plasticity # Yield condition Abaqus makes use of a composite yield surface to describe the different behavior in tension and compression. In tension yielding is assumed to be governed by the maximum principal stress, while in compression yielding is assumed to be pressure independent and governed by the deviatoric stresses alone (Mises yield condition). The model is described in detail in “Cast iron plasticity,” Section 4.3.7 of the Abaqus Theory Guide. # Flow rule For the purposes of discussing the flow and hardening behavior, it is useful to divide the meridional plane into the two regions shown in Figure 23.2.10–2. 

area

| Region | Mises stress, q | Equivalent pressure stress, p | | ------------------ | --------------- | ------------------------------ | | tensile region | G_t | 0 | | compressive region | G_c | 1 | | UC | 3 | 1 |

Figure 23.2.10–2 Schematic of the flow potentials in the p–q plane. The region to the left of the uniaxial compression line (labeled UC) is referred to as the “tensile region,” while the region to the right of the uniaxial compression line is referred to as the “compressive region.” The flow potential consists of the Mises cylinder in the compressive region and an ellipsoidal “cap” in the tensile region. The transition between the two surfaces is smooth. The projection of the flow potential on the meridional plane (see Figure 23.2.10–2) consists of a straight line in the compressive region and an ellipse in the tensile region. The corresponding projection on the deviatoric plane is a circle. A consequence of the above choice is that plastic flow results in inelastic volume expansion in the tensile region and no inelastic volume change in the compressive region (see “Cast iron plasticity,” Section 4.3.7 of the Abaqus Theory Guide, for details). # Nonassociated flow Since the flow potential is different from the yield surface (“nonassociated” flow), the material Jacobian matrix is unsymmetric. Hence, to improve convergence, use the unsymmetric matrix storage and solution scheme (see “Defining an analysis,” Section 6.1.2). # Hardening Since the hardening of gray cast iron is different in uniaxial tension and uniaxial compression, you need to provide two sets of hardening data in tabular form: one based on a uniaxial tension experiment that defines $\sigma _ { t } = \sigma _ { t } ( \bar { \varepsilon } _ { t } ^ { p l } , \theta , f ^ { \alpha } )$ and the other based on a uniaxial compression experiment that defines $\sigma _ { c } = \sigma _ { c } ( \bar { \varepsilon } _ { c } ^ { p l } , \theta , f ^ { \alpha } )$ . Here, $\bar { \varepsilon } _ { t } ^ { p l }$ and $\bar { \varepsilon } _ { c } ^ { p l }$ are the equivalent plastic strains in uniaxial tension and uniaxial compression, respectively. Input File Usage: Use both of the following options in conjunction with the \*CAST IRON PLASTICITY option: \*CAST IRON COMPRESSION HARDENING \*CAST IRON TENSION HARDENING Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Cast Iron Plasticity: Compression Hardening and Tension Hardening # Restrictions on material data The plastic Poisson’s ratio, $\nu _ { p l }$ , is expected to be less than 0.5 since experimental results suggest that there is a permanent increase in the volume of gray cast iron when it is loaded in uniaxial tension beyond yield. For the potential to be well-defined, $\nu _ { p l }$ must be greater than −1.0. Thus, the plastic Poisson’s ratio must satisfy $- 1 . 0 < \nu _ { p l } \leq 0 . 5$ . The cast iron plasticity material model is intended for modeling cast iron and other materials like cast iron for which the behavior in uniaxial tension and uniaxial compression matches the behavior shown in Figure 23.2.10–1. In particular, the model expects the initial yield stress in uniaxial tension to be less than the initial yield stress in uniaxial compression. Even if the overall stress-strain response and hardening behavior in uniaxial stress states of some material other than cast iron is consistent with that of cast iron, you must also ensure that the flow potential (which has been constructed specifically for modeling cast iron) for the model is meaningful for other materials. Abaqus issues a warning message only if the initial yield stress in uniaxial tension is equal to or greater than that in uniaxial compression. No other checks are carried out in this regard. If the yield stress in uniaxial tension is higher than that in uniaxial compression, a material point in uniaxial tension may actually yield at the initial yield stress specified for uniaxial compression. This apparent anomalous behavior is due to the fact that (as a result of unrealistic user-specified material properties) a uniaxial tension stressing path in stress space meets the compressive (Mises) part of the yield surface first. # Elements The cast iron plasticity model can be used with any stress/displacement element in Abaqus other than elements for which the assumed stress state is plane stress (plane stress continuum, shell, and membrane elements). It can be used with one-dimensional elements (trusses and beams in a plane) and, in Abaqus/Standard, with beams in space. # Output In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the cast iron plasticity material model: PEEQ Equivalent plastic strain in uniaxial compression, $\begin{array} { r } { \bar { \varepsilon } _ { c } ^ { p l } = \int _ { 0 } ^ { t } \dot { \bar { \varepsilon } } _ { c } ^ { p l } d t . } \end{array}$ . PEEQT Equivalent plastic strain in uniaxial tension, $\begin{array} { r } { \bar { \varepsilon } _ { t } ^ { p l } = \int _ { 0 } ^ { t } \dot { \bar { \varepsilon } } _ { t } ^ { p l } d t . } \end{array}$