Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
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,” Section 18.2.2.);
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,” Section 6.5.4) or an adiabatic thermal-stress analysis (“Adiabatic analysis,” Section 6.5.5) 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/Explicit (“Damage and failure for ductile metals: overview,” Section 19.2.1) 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,” Section 17.2.1) or the equation of state material model (“Equation of state,” Section 17.9.1).
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,” Section 18.2.9.
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: Mechanical |
The Hill yield surface allows anisotropic yielding to be modeled. You must specify a reference yield stress, 
, for the metal plasticity model and define a set of yield ratios, 
, separately. These data define the yield stress corresponding to each stress component as 
. Hill's potential function is discussed in detail in “Anisotropic yield/creep,” Section 18.2.6. Yield ratios can be used to define three common forms of anisotropy associated with sheet metal forming: transverse anisotropy, planar anisotropy, and general anisotropy.
| Input File Usage: | Use both of the following options: |
*PLASTIC (to specify the reference yield stress |
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
In ABAQUS a perfectly plastic material (with no hardening) can be defined, or work hardening can be specified. Isotropic hardening is available in both ABAQUS/Standard and ABAQUS/Explicit; Johnson-Cook hardening is available only in ABAQUS/Explicit. In addition, ABAQUS provides kinematic hardening for materials subjected to cyclic loading.
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: Mechanical |
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,” Section 4.3.2 of the ABAQUS Theory Manual.
If isotropic hardening is defined, the yield stress, , can be given as a tabular function of plastic strain and, if required, of temperature and/or other predefined field variables. The yield stress at a given state is simply interpolated from this table of data, and it remains constant for plastic strains exceeding the last value given as tabular data.
ABAQUS/Explicit will regularize 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,” Section 16.1.2, for a more detailed discussion of data regularization.
| Input File Usage: | *PLASTIC, HARDENING=ISOTROPIC (default if parameter is omitted) |
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
Johnson-Cook hardening is a particular type of isotropic hardening in ABAQUS/Explicit 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 “Anisotropic yield/creep,” Section 18.2.6) cannot be used with Johnson-Cook hardening. For more details, see “Johnson-Cook plasticity,” Section 18.2.7.
| Input File Usage: | *PLASTIC, HARDENING=JOHNSON COOK |
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
In ABAQUS/Standard the yield stress for isotropic hardening, , can alternatively be described through user subroutine UHARD.
| Input File Usage: | *PLASTIC, HARDENING=USER |
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
Two 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. For more details, see “Models for metals subjected to cyclic loading,” Section 18.2.2.
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
The combined hardening model is not supported in ABAQUS/CAE. |
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.
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.
Test data can be provided as tables of yield stress values versus equivalent plastic strain at different equivalent plastic strain rates (
); 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,” Section 18.2.3.
| Input File Usage: | *PLASTIC, RATE= |
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
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
is the static yield stress, 
is the equivalent plastic strain, is the equivalent plastic strain rate, and R is a ratio, defined as 
at 
. This method is described further in “Rate-dependent yield,” Section 18.2.3.| Input File Usage: | Use both of the following options: |
*PLASTIC (to specify the static yield stress |
| ABAQUS/CAE Usage: | Property module: material editor: Mechanical |
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: Mechanical |
In ABAQUS/Explicit the metal plasticity material models can be used in conjunction with the progressive damage and failure models discussed in “Damage and failure for ductile metals: overview,” Section 19.2.1. 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 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: Mechanical Damage for Ductile Metalscriterion: SuboptionsDamage Evolution |
In ABAQUS/Explicit the metal plasticity material models can be used in conjunction with the shear and tensile failure models (“Dynamic failure models,” Section 18.2.8) that are applicable in truly dynamic situations; however, the progressive damage and failure models discussed above are generally preferred.
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,” Section 18.2.8.
| 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. |
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,” Section 18.2.8.
| Input File Usage: | Use both of the following options: |
*PLASTIC *TENSILE FAILURE |
| ABAQUS/CAE Usage: | The tensile failure model is not supported in ABAQUS/CAE. |
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,” Section 6.5.5) or fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.4).
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: |
There are cases when we need to study the behavior of a material that has already been subjected to some work hardening. For such cases initial equivalent plastic strain values can be provided to specify the yield stress corresponding to the work hardened state (see “Initial conditions,” Section 27.2.1).
| Input File Usage: | *INITIAL CONDITIONS, TYPE=HARDENING |
| ABAQUS/CAE Usage: | Initial equivalent plastic strain is not supported in ABAQUS/CAE. |
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: | User subroutine HARDINI is not supported in ABAQUS/CAE. |
Classical metal plasticity can be used with any elements that include mechanical behavior (elements that have displacement degrees of freedom).
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 variable has special meaning for the classical metal plasticity models:
PEEQ | Equivalent plastic strain, |
)
)
where 
is the initial equivalent plastic strain (zero or user-specified; see