Classical Metal Plasticity

The Mises yield surface is used to define isotropic yielding. It is defined by giving the value of the uniaxial yield stress as a function of uniaxial equivalent plastic strain, temperature, and/or field variables. In Abaqus/Standard the yield stress can alternatively be defined in user subroutine UHARD.

PLASTIC

Property module: material editor: MechanicalPlasticityPlastic

The quadratic Hill yield surface allows anisotropic yielding to be modeled. You must specify a reference yield stress, ${\sigma }^0$, for the metal plasticity model and define a set of yield ratios, $R_{ij}$, separately. These data define the yield stress corresponding to each stress component as $R_{ij}{\sigma }^0$. Hill's potential function is discussed in detail in Hill Anisotropic Yield/Creep. Yield ratios can be used to define three common forms of anisotropy associated with sheet metal forming: transverse anisotropy, planar anisotropy, and general anisotropy.

The plasticity model using the Hill yield surface is applicable to strains up to about 25%–30%, and it is not recommended for analyses in which these values are exceeded.

PLASTIC (to specify the reference yield stress, ${\sigma }^0$)
POTENTIAL, TYPE=HILL (default)  (to specify the yield ratios, $R_{ij}$)

Property module: material editor: MechanicalPlasticityPlastic: SuboptionsPotential

Perfect plasticity means that the yield stress does not change with plastic strain. It can be defined in tabular form for a range of temperatures and/or field variables; a single yield stress value per temperature and/or field variable specifies the onset of yield.

PLASTIC

Property module: material editor: MechanicalPlasticityPlastic

Isotropic hardening means that the yield surface changes size uniformly in all directions such that the yield stress increases (or decreases) in all stress directions as plastic straining occurs. Abaqus provides an isotropic hardening model, which is useful for cases involving gross plastic straining or in cases where the straining at each point is essentially in the same direction in strain space throughout the analysis. Although the model is referred to as a “hardening” model, strain softening or hardening followed by softening can be defined. Isotropic hardening plasticity is discussed in more detail in Isotropic elasto-plasticity.

If isotropic hardening is defined, the yield stress, ${\sigma }^0$ , can be given as a tabular function of equivalent plastic strain and, if required, of temperature and/or other predefined field variables. The yield stress at a given state is interpolated from this table of data, and it is assumed to remain constant outside the range of the independent variables other than equivalent plastic strain. Outside the range of equivalent plastic strains, you can choose if the yield stress remains constant (default) or is extrapolated linearly (see Extrapolation of Material Data).

Abaqus/Explicit regularizes the data into tables that are defined in terms of even intervals of the independent variables. In some cases where the yield stress is defined at uneven intervals of the independent variable (plastic strain) and the range of the independent variable is large compared to the smallest interval, Abaqus/Explicit may fail to obtain an accurate regularization of your data in a reasonable number of intervals. In this case the program will stop after all data are processed with an error message that you must redefine the material data. See Material Data Definition for a more detailed discussion of data regularization.

PLASTIC, HARDENING=ISOTROPIC (default if parameter is omitted)

PLASTIC, EXTRAPOLATION=CONSTANT (default)

PLASTIC, EXTRAPOLATION=LINEAR

Property module: material editor: MechanicalPlasticityPlastic: Hardening: Isotropic: Extrapolation: Constant or Linear

Johnson-Cook hardening is a particular type of isotropic hardening where the yield stress is given as an analytical function of equivalent plastic strain, strain rate, and temperature. This hardening law is suited for modeling high-rate deformation of many materials including most metals. Hill's potential function (see Hill Anisotropic Yield/Creep) cannot be used with Johnson-Cook hardening. For more details, see Johnson-Cook Plasticity.

PLASTIC, HARDENING=JOHNSON COOK

Property module: material editor: MechanicalPlasticityPlastic: Hardening: Johnson-Cook

In Abaqus/Standard the yield stress for isotropic hardening, ${\sigma }^0$, can alternatively be described through user subroutine UHARD.

PLASTIC, HARDENING=USER

Property module: material editor: MechanicalPlasticityPlastic: Hardening: User

Three kinematic hardening models are provided in Abaqus to model the cyclic loading of metals. The linear kinematic model approximates the hardening behavior with a constant rate of hardening. The more general nonlinear isotropic/kinematic model will give better predictions but requires more detailed calibration. The multilinear kinematic model combines several piecewise linear hardening curves to predict the complex response of metals under thermomechanical load cycles. This model is based on Besseling (1958) and is available only in Abaqus/Standard. For more details, see Models for Metals Subjected to Cyclic Loading.

PLASTIC, HARDENING=KINEMATIC

PLASTIC, HARDENING=COMBINED

PLASTIC, HARDENING=MULTILINEAR KINEMATIC

Property module: material editor: MechanicalPlasticityPlastic: Hardening: Kinematic or Multilinear-Kinematic or Combined

Test data can be provided as tables of yield stress values versus equivalent plastic strain at different equivalent plastic strain rates (${\dot{\overline{\epsilon }}}^{pl}$); one table per strain rate. Direct tabular data cannot be used with Johnson-Cook hardening. The guidelines that govern the entry of this data are provided in Rate-Dependent Yield.

PLASTIC, RATE=${\dot{\overline{\epsilon }}}^{pl}$

Property module: material editor: MechanicalPlasticityPlastic: Use strain-rate-dependent data

Alternatively, you can specify the strain rate dependence by means of a scaling function. In this case you enter only one hardening curve, the static hardening curve, and then express the rate-dependent hardening curves in terms of the static relation; that is, we assume that

where ${\sigma }^0$ is the static yield stress, ${\overline{\epsilon }}^{pl}$ is the equivalent plastic strain, ${\dot{\overline{\epsilon }}}^{pl}$ is the equivalent plastic strain rate, and R is a ratio, defined as $R=1.0$ at ${\dot{\overline{\epsilon }}}^{pl}=0.0$. This method is described further in Rate-Dependent Yield.

PLASTIC (to specify the static yield stress ${\sigma }^0\left({\overline{\epsilon }}^{pl}\right)$)
RATE DEPENDENT (to specify the ratio $R\left({\dot{\overline{\epsilon }}}^{pl}\right)$)

Property module: material editor: MechanicalPlasticityPlastic: SuboptionsRate Dependent

In Abaqus/Standard user subroutine UHARD can be used to define a rate-dependent yield stress. You are provided the current equivalent plastic strain and equivalent plastic strain rate and are responsible for returning the yield stress and derivatives.

PLASTIC, HARDENING=USER

Property module: material editor: MechanicalPlasticityPlastic: Hardening: User

The shear failure model provides a simple failure criterion that is suitable for high-strain-rate deformation of many materials including most metals. It offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The shear failure criterion is based on the value of the equivalent plastic strain and is applicable mainly to high-strain-rate, truly dynamic problems. For more details, see Dynamic Failure Models.

PLASTIC
SHEAR FAILURE

The tensile failure model uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff. It offers a number of failure choices including element removal. Similarly to the shear failure model, the tensile failure model is suitable for high-strain-rate deformation of metals and is applicable to truly dynamic problems. For more details, see Dynamic Failure Models.

PLASTIC
TENSILE FAILURE

Property module: material editor: MechanicalPlasticityPlastic: SuboptionsTensile Failure

For more complicated cases, initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI.

INITIAL CONDITIONS, TYPE=HARDENING, USER

Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined