Processing math: 100%

Classical Metal Plasticity

The classical metal plasticity models:

use Mises or Hill yield surfaces with associated plastic flow, which allow for isotropic and anisotropic yield, respectively;
use perfect plasticity or isotropic hardening behavior;
can be used when rate-dependent effects are important;
are intended for applications such as crash analyses, metal forming, and general collapse studies (Plasticity models that include kinematic hardening and are, therefore, more suitable for cases involving cyclic loading are also available in Abaqus: see Models for Metals Subjected to Cyclic Loading.);
can be used in any procedure that uses elements with displacement degrees of freedom;
can be used in a fully coupled temperature-displacement analysis (Fully Coupled Thermal-Stress Analysis), a fully coupled thermal-electrical-structural analysis (Fully Coupled Thermal-Electrical-Structural Analysis), or an adiabatic thermal-stress analysis (Adiabatic Analysis) such that plastic dissipation results in the heating of a material;
can be used in conjunction with the models of progressive damage and failure in Abaqus (About Damage and Failure for Ductile Metals) to specify different damage initiation criteria and damage evolution laws that allow for the progressive degradation of the material stiffness and the removal of elements from the mesh;
can be used in conjunction with the shear failure model in Abaqus/Explicit to provide a simple ductile dynamic failure criterion that allows for the removal of elements from the mesh, although the progressive damage and failure methods discussed above are generally recommended instead;
can be used in conjunction with the tensile failure model in Abaqus/Explicit to provide a tensile spall criterion offering a number of failure choices and removal of elements from the mesh; and
must be used in conjunction with either the linear elastic material model (Linear Elastic Behavior) or the equation of state material model (Equation of State).

This page discusses:

Yield Surfaces
Hardening
Flow Rule
Rate Dependence
Progressive Damage and Failure
Shear and Tensile Dynamic Failure in Abaqus/Explicit
Heat Generation by Plastic Work
Initial Conditions
Elements
Output
References

Yield Surfaces

The Mises and Hill yield surfaces assume that yielding of the metal is independent of the equivalent pressure stress: this observation is confirmed experimentally for most metals (except voided metals) under positive pressure stress but may be inaccurate for metals under conditions of high triaxial tension when voids may nucleate and grow in the material. Such conditions can arise in stress fields near crack tips and in some extreme thermal loading cases such as those that might occur during welding processes. A porous metal plasticity model is provided in Abaqus for such situations. This model is described in Porous Metal Plasticity.

Mises Yield Surface

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.

Input File Usage

PLASTIC

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic

Hill Yield Surface

The quadratic Hill yield surface allows anisotropic yielding to be modeled. You must specify a reference yield stress, $σ^{0}$ , for the metal plasticity model and define a set of yield ratios, $R_{i j}$ , separately. These data define the yield stress corresponding to each stress component as $R_{i j} σ^{0}$ . 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.

Input File Usage

Use both of the following options:

PLASTIC (to specify the reference yield stress,  $σ^{0}$ )
POTENTIAL, TYPE=HILL (default)  (to specify the yield ratios,  $R_{i j}$ )

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic: SuboptionsPotential

Hardening

In Abaqus a perfectly plastic material (with no hardening) can be defined, or work hardening can be specified. Isotropic hardening, including Johnson-Cook hardening, is available in both Abaqus/Standard and Abaqus/Explicit. In addition, Abaqus provides kinematic hardening for materials subjected to cyclic loading.

Perfect Plasticity

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.

Input File Usage

PLASTIC

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic

Isotropic Hardening

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, $σ^{0}$ , 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.

Input File Usage

Use the following option to define isotropic hardening with tabular data:

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

Use the following option to request that the yield stress remains constant outside the specified range of the equivalent plastic strains:

PLASTIC, EXTRAPOLATION=CONSTANT (default)

Use the following option to request linear extrapolation of the yield stress outside the specified range of the equivalent plastic strains:

PLASTIC, EXTRAPOLATION=LINEAR

Abaqus/CAE Usage

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

Johnson-Cook Isotropic Hardening

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.

Input File Usage

PLASTIC, HARDENING=JOHNSON COOK

Abaqus/CAE Usage

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

User Subroutine

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

Input File Usage

PLASTIC, HARDENING=USER

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic: Hardening: User

Kinematic Hardening

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.

Input File Usage

Use the following option to specify the linear kinematic model:

PLASTIC, HARDENING=KINEMATIC

Use the following option to specify the nonlinear combined isotropic/kinematic model:

PLASTIC, HARDENING=COMBINED

Use the following option to specify the multilinear kinematic hardening model:

PLASTIC, HARDENING=MULTILINEAR KINEMATIC

Abaqus/CAE Usage

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

Flow Rule

Abaqus uses associated plastic flow. Therefore, as the material yields, the inelastic deformation rate is in the direction of the normal to the yield surface (the plastic deformation is volume invariant). This assumption is generally acceptable for most calculations with metals; the most obvious case where it is not appropriate is the detailed study of the localization of plastic flow in sheets of metal as the sheet develops texture and eventually tears apart. So long as the details of such effects are not of interest (or can be inferred from less detailed criteria, such as reaching a forming limit that is defined in terms of strain), the associated flow models in Abaqus used with the smooth Mises or Hill yield surfaces generally predict the behavior accurately.

Rate Dependence

As strain rates increase, many materials show an increase in their yield strength. This effect becomes important in many metals when the strain rates range between 0.1 and 1 per second; and it can be very important for strain rates ranging between 10 and 100 per second, which are characteristic of high-energy dynamic events or manufacturing processes.

There are multiple ways to introduce a strain-rate-dependent yield stress.

Direct Tabular Data

Test data can be provided as tables of yield stress values versus equivalent plastic strain at different equivalent plastic strain rates ( ${\dot{\bar{ε}}}^{p l}$ ); 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.

Input File Usage

PLASTIC, RATE= ${\dot{\bar{ε}}}^{p l}$

Abaqus/CAE Usage

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

Yield Stress Ratios

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

$\bar{σ} ({\bar{ε}}^{p l}, {\dot{\bar{ε}}}^{p l}) = σ^{0} ({\bar{ε}}^{p l}) R ({\dot{\bar{ε}}}^{p l}),$

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

Input File Usage

Use both of the following options:

PLASTIC (to specify the static yield stress  $σ^{0} ({\bar{ε}}^{p l})$ )
RATE DEPENDENT (to specify the ratio  $R ({\dot{\bar{ε}}}^{p l})$ )

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic: SuboptionsRate Dependent

User Subroutine

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.

Input File Usage

PLASTIC, HARDENING=USER

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic: Hardening: User

Progressive Damage and Failure

In Abaqus the metal plasticity material models can be used in conjunction with the progressive damage and failure models discussed in About Damage and Failure for Ductile Metals. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), Müschenborn-Sonne forming limit diagram (MSFLD), and, in Abaqus/Explicit, Marciniak-Kuczynski (M-K) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The model offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations. This is a great advantage over the dynamic failure models discussed next.

Input File Usage

Use the following options:

PLASTIC
DAMAGE INITIATION
DAMAGE EVOLUTION

Abaqus/CAE Usage

Property module: material editor: MechanicalDamage for Ductile Metalscriterion: SuboptionsDamage Evolution

Shear and Tensile Dynamic Failure in Abaqus/Explicit

In Abaqus/Explicit the metal plasticity material models can be used in conjunction with the shear and tensile failure models (Dynamic Failure Models) that are applicable in truly dynamic situations; however, the progressive damage and failure models discussed above are generally preferred.

Shear Failure

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.

Input File Usage

Use both of the following options:

PLASTIC
SHEAR FAILURE

Abaqus/CAE Usage

The shear failure model is not supported in Abaqus/CAE.

Tensile 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.

Input File Usage

Use both of the following options:

PLASTIC
TENSILE FAILURE

Abaqus/CAE Usage

Property module: material editor: MechanicalPlasticityPlastic: SuboptionsTensile Failure

Heat Generation by Plastic Work

Abaqus optionally allows for plastic dissipation to result in the heating of a material. Heat generation is typically used in the simulation of bulk metal forming or high-speed manufacturing processes involving large amounts of inelastic strain where the heating of the material caused by its deformation is an important effect because of temperature dependence of the material properties. It is applicable only to adiabatic thermal-stress analysis (Adiabatic Analysis), fully coupled temperature-displacement analysis (Fully Coupled Thermal-Stress Analysis), or fully coupled thermal-electrical-structural analysis (Fully Coupled Thermal-Electrical-Structural Analysis).

This effect is introduced by defining the fraction of the rate of inelastic dissipation that appears as a heat flux per volume.

Input File Usage

Use all of the following options in the same material data block:

PLASTIC
SPECIFIC HEAT
DENSITY
INELASTIC HEAT FRACTION

Abaqus/CAE Usage

Use all of the following options for the same material:

Property module: material editor: 
MechanicalPlasticityPlastic
ThermalSpecific Heat
GeneralDensity
ThermalInelastic Heat Fraction

Initial Conditions

When we need to study the behavior of a material that has already been subjected to some work hardening, initial equivalent plastic strain values can be provided to specify the yield stress corresponding to the work hardened state (see Initial Conditions).

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

User Subroutine Specification in Abaqus/Standard

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

Classical metal plasticity can be used with any elements that include mechanical behavior (elements that have displacement degrees of freedom).

Output

In 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 for the classical metal plasticity models:

PEEQ: Equivalent plastic strain, ${\bar{ε}}^{p l} = {{\bar{ε}}^{p l} |}_{0} + \int_{0}^{t} \sqrt{\frac{2}{3} {\dot{ε}}^{p l} : {\dot{ε}}^{p l}} d t,$ where ${{\bar{ε}}^{p l} |}_{0}$ is the initial equivalent plastic strain (zero or user-specified; see Initial Conditions).
YIELDS: Yield stress, $σ^{0}$ .

References

Besseling, J. F., “A Theory of Elastic, Plastic, and Creep Deformations of an Initially Isotropic Material Showing Anisotropic Strain-Hardening, Creep Recovery, and Secondary Creep,” Journal of Applied Mechanics, pp. 529–536, 1958.