ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE Elastic and plastic behaviorYou specify the elastic part of the response separately; only linear isotropic elasticity can be specified (see Linear elastic behavior). The porous metal plasticity model cannot be used in conjunction with porous elasticity (Elastic behavior of porous materials). You specify the hardening behavior of the fully dense matrix material by defining a metal plasticity model (see Classical metal plasticity). Only isotropic hardening can be specified. The hardening curve must describe the yield stress of the matrix material as a function of plastic strain in the matrix material. In defining this dependence at finite strains, “true” (Cauchy) stress and log strain values should be given. Rate dependency effects for the matrix material can be modeled (see Ratedependent yield). Yield conditionThe relative density of a material, r, is defined as the ratio of the volume of solid material to the total volume of the material. The relationships defining the model are expressed in terms of the void volume fraction, f, which is defined as the ratio of the volume of voids to the total volume of the material. It follows that $f=1r.$ For a metal containing a dilute concentration of voids, Gurson (1977) proposed a yield condition as a function of the void volume fraction. This yield condition was later modified by Tvergaard (1981) to the form $$\mathrm{\Phi}={\left(\frac{q}{{\sigma}_{y}}\right)}^{2}+2{q}_{1}f\mathrm{cosh}\left({q}_{2}\frac{3p}{2{\sigma}_{y}}\right)\left(1+{q}_{3}{f}^{2}\right)=0,$$ where
The Cauchy stress is defined as the force per “current unit area,” comprised of voids and the solid (matrix) material. f = 0 (r = 1) implies that the material is fully dense, and the Gurson yield condition reduces to the Mises yield condition. f = 1 (r = 0) implies that the material is completely voided and has no stress carrying capacity. The model generally gives physically reasonable results only for $f<$0.1 ($r>$0.9). The model is described in detail in Porous metal plasticity, along with a discussion of its numerical implementation. If the porous metal plasticity model is used during a pore pressure analysis (see Coupled pore fluid diffusion and stress analysis), the relative density, r, is tracked independently of the void ratio. Specifying q_{1}, q_{2}, and q_{3}You specify the parameters ${q}_{1}$, ${q}_{2}$, and ${q}_{3}$ directly for the porous metal plasticity model. For typical metals the ranges of the parameters reported in the literature are ${q}_{1}$ = 1.0 to 1.5, ${q}_{2}$ = 1.0, and ${q}_{3}$ = ${q}_{1}^{2}$ = 1.0 to 2.25 (see Necking of a round tensile bar). The original Gurson model is recovered when ${q}_{1}$ = ${q}_{2}$ = ${q}_{3}$ = 1.0. You can define these parameters as tabular functions of temperature and/or field variables. Input File Usage POROUS METAL PLASTICITY Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityPorous Metal Plasticity Failure criteria in Abaqus/ExplicitThe porous metal plasticity model in Abaqus/Explicit allows for failure. In this case the yield condition is written as $$\mathrm{\Phi}={\left(\frac{q}{{\sigma}_{y}}\right)}^{2}+2{q}_{1}{f}^{*}\mathrm{cosh}\left({q}_{2}\frac{3p}{2{\sigma}_{y}}\right)\left(1+{q}_{3}f^{*}{}^{2}\right)=0,$$ where the function ${f}^{*}\left(f\right)$ models the rapid loss of stress carrying capacity that accompanies void coalescence. This function is defined in terms of the void volume fraction: $${f}^{*}=\{\begin{array}{c}f\text{if}f\le {f}_{c},\hfill \\ {f}_{c}+\frac{{\overline{f}}_{F}{f}_{c}}{{f}_{F}{f}_{c}}\left(f{f}_{c}\right)\text{if}{f}_{c}f{f}_{F}\hfill \\ {\overline{f}}_{F}\text{if}f\ge {f}_{F}\text{,}\hfill \end{array},$$ where $${\overline{f}}_{F}=\frac{{q}_{1}+\sqrt{{q}_{1}^{2}{q}_{3}}}{{q}_{3}}.$$ 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 $f\ge {f}_{F}$, 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: MechanicalPlasticityPorous Metal Plasticity: SuboptionsPorous Failure Criteria Specifying the initial relative densityYou 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 pointsYou can specify the initial relative density as part of the porous metal plasticity material definition. Input File Usage POROUS METAL PLASTICITY, RELATIVE DENSITY=${r}_{0}$ Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityPorous Metal Plasticity: Relative density: ${r}_{0}$ At nodesAlternatively, you can specify the initial relative density at nodes as initial conditions (Initial conditions in Abaqus/Standard and Abaqus/Explicit); 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 multipoint 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 hardeningThe presence of pressure in the yield condition results in nondeviatoric plastic strains. Plastic flow is assumed to be normal to the yield surface: $${\dot{\mathit{\epsilon}}}^{pl}=\dot{\lambda}\frac{\partial \mathrm{\Phi}}{\partial \mathit{\sigma}}.$$ The hardening of the fully dense matrix material is described through ${\sigma}_{y}={\sigma}_{y}\left({\overline{\epsilon}}_{m}^{pl}\right)$. The evolution of the equivalent plastic strain in the matrix material is obtained from the following equivalent plastic work expression: $$\left(1f\right){\sigma}_{y}{\dot{\overline{\epsilon}}}_{m}^{pl}=\mathit{\sigma}:{\dot{\mathit{\epsilon}}}^{pl}.$$ The model is illustrated in Figure 1, where the yield surfaces for different levels of void volume fraction are shown in the p–q plane. Figure 1. Schematic of the yield surface in the
p–q plane.
Figure 2 compares the behavior of a porous material (whose initial yield stress is ${\sigma}_{{y}_{0}}$) in 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. Figure 2. Schematic of uniaxial behavior of a porous metal (perfectly plastic
matrix material with initial volume fraction of voids =
${f}_{0}$).
Void growth and nucleationThe total change in void volume fraction is given as $$\dot{f}={\dot{f}}_{\mathrm{gr}}+{\dot{f}}_{\mathrm{nucl}},$$ where ${\dot{f}}_{\mathrm{gr}}$ is change due to growth of existing voids and ${\dot{f}}_{\mathrm{nucl}}$ 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: $${\dot{f}}_{\mathrm{gr}}=\left(1f\right){\dot{\mathit{\epsilon}}}^{pl}:\mathbf{I}.$$ The nucleation of voids is given by a straincontrolled relationship: $${\dot{f}}_{\mathrm{nucl}}=A{\dot{\overline{\epsilon}}}_{m}^{pl},$$ where $$A=\frac{{f}_{N}}{{s}_{N}\sqrt{2\pi}}\mathrm{exp}\left[\frac{1}{2}{\left(\frac{{\overline{\epsilon}}_{m}^{pl}{\epsilon}_{N}}{{s}_{N}}\right)}^{2}\right].$$ The normal distribution of the nucleation strain has a mean value ${\epsilon}_{N}$ 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 3 for different values of the standard deviation ${s}_{N}$. Figure 3. Nucleation function $A/{f}_{N}$.
Figure 4 shows the extent of softening in a uniaxial tension test of a porous material for different values of ${f}_{N}$. Figure 4. Softening (in uniaxial tension) as a function of
${f}_{N}$.
The following ranges of values are reported in the literature for typical metals: ${\epsilon}_{N}$ = 0.1 to 0.3, ${s}_{N}=$ 0.05 to 0.1, and ${f}_{N}$ = 0.04 (see Necking of a round tensile bar). 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: MechanicalPlasticityPorous Metal Plasticity: SuboptionsVoid Nucleation Initial conditionsWhen 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, ${\overline{\epsilon}}^{pl}$ (Initial conditions in Abaqus/Standard and Abaqus/Explicit). 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 subroutineFor 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: Userdefined ElementsThe 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). OutputIn addition to the standard output identifiers available in Abaqus (Abaqus/Standard output variable identifiers and Abaqus/Explicit output variable identifiers), the following variables have special meaning in the porous metal plasticity model:
References
