 Classical metal plasticity

The yield and inelastic flow of a metal at relatively low temperatures,
where loading is relatively monotonic and creep effects are not important, can
typically be described with the classical metal plasticity models (Classical metal plasticity).
In
Abaqus
these models use standard Mises or Hill yield surfaces with associated plastic
flow. Perfect plasticity and isotropic hardening definitions are both available
in the classical metal plasticity models. Common applications include crash
analyses, metal forming, and general collapse studies; the models are simple
and adequate for such cases.
 Models for metals
subjected to cyclic loading

A linear kinematic hardening model or a nonlinear isotropic/kinematic
hardening model (Models for metals subjected to cyclic loading)
can be used in
Abaqus
to simulate the behavior of materials that are subjected to cyclic loading. The
evolution law in these models consists of a kinematic hardening component
(which describes the translation of the yield surface in stress space) and, for
the nonlinear isotropic/kinematic hardening model, of an isotropic component
(which describes the change of the elastic range). The Bauschinger effect and
plastic shakedown can be modeled with both models, but the nonlinear
isotropic/kinematic hardening model provides more accurate predictions.
Ratchetting and relaxation of the mean stress are accounted for only by the
nonlinear isotropic/kinematic model. In addition to these two models, the
ORNL model in
Abaqus/Standard
can be used when simple life estimation is desired for the design of stainless
steels subjected to lowcycle fatigue and creep fatigue (see below).
 Ratedependent
yield

As strain rates increase, many materials show an increase in their yield
strength. Rate dependence (Ratedependent yield)
can be defined in
Abaqus
for a number of plasticity models. Rate dependence can be used in both static
and dynamic procedures. Applicable models include classical metal plasticity,
extended DruckerPrager plasticity, and crushable foam plasticity.
 Creep and
swelling

Abaqus/Standard
provides a material model for classical metal creep behavior and timedependent
volumetric swelling behavior (Ratedependent plasticity: creep and swelling).
This model is intended for relatively slow (quasistatic) inelastic deformation
of a model such as the hightemperature creeping flow of a metal or a piece of
glass. The creep strain rate is assumed to be purely deviatoric, meaning that
there is no volume change associated with this part of the inelastic straining.
Creep can be used with the classical metal plasticity model, with the
ORNL model, and to define ratedependent
gasket behavior (Defining the gasket behavior directly using a gasket behavior model).
Swelling can be used with the classical metal plasticity model. (Usage with the
DruckerPrager models is explained below.)
 Annealing or
melting

Abaqus
provides a modeling capability for situations in which a loss of memory related
to hardening occurs above a certain userdefined temperature, known as the
annealing temperature (Annealing or melting).
It is intended for use with metals subjected to hightemperature deformation
processes, in which the material may undergo melting and possibly
resolidification or some other form of annealing. In
Abaqus
annealing or melting can be modeled with classical metal plasticity (Mises and
Hill); in
Abaqus/Explicit
annealing or melting can also be modeled with JohnsonCook plasticity. The
annealing temperature is assumed to be a material property. See
Annealing
for information on an alternative method for simulating annealing in
Abaqus/Explicit.
 Anisotropic yield
and creep

Abaqus
provides an anisotropic yield model (Anisotropic yield/creep),
which is available for use with materials modeled with classical metal
plasticity (Classical metal plasticity),
kinematic hardening (Models for metals subjected to cyclic loading),
and/or creep (Ratedependent plasticity: creep and swelling)
that exhibit different yield stresses in different directions. The
Abaqus/Standard
model includes creep; creep behavior is not available in
Abaqus/Explicit.
The model allows for the specification of different stress ratios for each
stress component to define the initial anisotropy. The model is not adequate
for cases in which the anisotropy changes significantly as the material deforms
as a result of loading.
 JohnsonCook
plasticity

The JohnsonCook plasticity model in
Abaqus/Explicit
(JohnsonCook plasticity)
is particularly suited to model highstrainrate deformation of metals. This
model is a particular type of Mises plasticity that includes analytical forms
of the hardening law and rate dependence. It is generally used in adiabatic
transient dynamic analysis.
 Dynamic failure
models

Two types of dynamic failure models are offered in
Abaqus/Explicit
for the Mises and JohnsonCook plasticity models (Dynamic failure models).
One is the shear failure model, where the failure criterion is based on the
accumulated equivalent plastic strain. Another is the tensile failure model,
which uses the hydrostatic pressure stress as a failure measure to model
dynamic spall or a pressure cutoff. Both models offer a number of failure
choices including element removal and are applicable mainly in truly dynamic
situations. In contrast, the progressive failure and damage models (Progressive Damage and Failure)
are suitable for both quasistatic and dynamic situations and have other
significant advantages.
 Porous metal
plasticity

The porous metal plasticity model (Porous metal plasticity)
is used to model materials that exhibit damage in the form of void initiation
and growth, and it can also be used for some powder metal process simulations
at high relative densities (relative density is defined as the ratio of the
volume of solid material to the total volume of the material). The model is
based on Gurson's porous metal plasticity theory with void nucleation and is
intended for use with materials that have a relative density that is greater
than 0.9. The model is adequate for relatively monotonic loading.
 Cast iron
plasticity

The cast iron plasticity model (Cast iron plasticity)
is used to model gray cast iron, which exhibits markedly different inelastic
behavior in tension and compression. The microstructure of gray cast iron
consists of a distribution of graphite flakes in a steel matrix. In tension the
graphite flakes act as stress concentrators, while in compression the flakes
serve to transmit stresses. The resulting material is brittle in tension, but
in compression it is similar in behavior to steel. The differences in tensile
and compressive plastic response include: (i) a yield stress in tension that is
three to five times lower than the yield stress in compression; (ii) permanent
volume increase in tension, but negligible inelastic volume change in
compression; (iii) different hardening behavior in tension and compression. The
model is adequate for relatively monotonic loading.
 Twolayer
viscoplasticity

The twolayer viscoplasticity model in
Abaqus/Standard
(Twolayer viscoplasticity)
is useful for modeling materials in which significant timedependent behavior
as well as plasticity is observed. For metals this typically occurs at elevated
temperatures. The model has been shown to provide good results for
thermomechanical loading.
 ORNL constitutive
model

The ORNL plasticity model in
Abaqus/Standard (ORNL – Oak Ridge National Laboratory constitutive model)
is intended for cyclic loading and hightemperature creep of type 304 and 316
stainless steel. Plasticity and creep calculations are provided according to
the specification in Nuclear Standard NEF
95T, “Guidelines and Procedures for Design of Class I Elevated Temperature
Nuclear System Components.” This model is an extension of the linear kinematic
hardening model (discussed above), which attempts to provide for simple life
estimation for design purposes when lowcycle fatigue and creep fatigue are
critical issues.
 Deformation
plasticity

Abaqus/Standard
provides a deformation theory RambergOsgood plasticity model (Deformation plasticity)
for use in developing fully plastic solutions for fracture mechanics
applications in ductile metals. The model is most commonly applied in static
loading with smalldisplacement analysis for which the fully plastic solution
must be developed in a part of the model.
 Extended
DruckerPrager plasticity and creep

The extended DruckerPrager family of plasticity models (Extended DruckerPrager models)
describes the behavior of granular materials or polymers in which the yield
behavior depends on the equivalent pressure stress. The inelastic deformation
may sometimes be associated with frictional mechanisms such as sliding of
particles across each other.
This class of models provides a choice of three different yield criteria.
The differences in criteria are based on the shape of the yield surface in the
meridional plane, which can be a linear form, a hyperbolic form, or a general
exponent form. Inelastic timedependent (creep) behavior coupled with the
plastic behavior is also available in
Abaqus/Standard
for the linear form of the model. Creep behavior is not available in
Abaqus/Explicit.
 Modified
DruckerPrager/Cap plasticity and creep

The modified DruckerPrager/Cap plasticity model (Modified DruckerPrager/Cap model)
can be used to simulate geological materials that exhibit pressuredependent
yield. The addition of a cap yield surface helps control volume dilatancy when
the material yields in shear and provides an inelastic hardening mechanism to
represent plastic compaction. In
Abaqus/Standard
inelastic timedependent (creep) behavior coupled with the plastic behavior is
also available for this model; two creep mechanisms are possible: a cohesion,
DruckerPragerlike mechanism and a consolidation, caplike mechanism.
 MohrCoulomb
plasticity

The MohrCoulomb plasticity model (MohrCoulomb plasticity)
can be used for design applications in the geotechnical engineering area. The
model uses the classical MohrColoumb yield criterion: a straight line in the
meridional plane and an irregular hexagonal section in the deviatoric plane.
However, the
Abaqus
MohrCoulomb model has a completely smooth flow potential instead of the
classical hexagonal pyramid: the flow potential is a hyperbola in the
meridional plane, and it uses the smooth deviatoric section proposed by
Menétrey and Willam.
 Critical state
(clay) plasticity

The clay plasticity model (Critical state (clay) plasticity model)
describes the inelastic response of cohesionless soils. The model provides a
reasonable match to the experimentally observed behavior of saturated clays.
This model defines the inelastic behavior of a material by a yield function
that depends on the three stress invariants, an associated flow assumption to
define the plastic strain rate, and a strain hardening theory that changes the
size of the yield surface according to the inelastic volumetric strain.
 Crushable foam
plasticity

The foam plasticity model (Crushable foam plasticity models)
is intended for modeling crushable foams that are typically used as energy
absorption structures; however, other crushable materials such as balsa wood
can also be simulated with this model. This model is most appropriate for
relatively monotonic loading. The crushable foam model with isotropic hardening
is applicable to polymeric foams as well as metallic foams.
 Jointed
material

The jointed material model in
Abaqus/Standard (Jointed material model)
is intended to provide a simple, continuum model for a material that contains a
high density of parallel joint surfaces in different orientations, such as
sedimentary rock. This model is intended for applications where stresses are
mainly compressive, and it provides a joint opening capability when the stress
normal to the joint tries to become tensile.
 Concrete

Three different constitutive models are offered in
Abaqus
for the analysis of concrete at low confining pressures: the smeared crack
concrete model in
Abaqus/Standard
(Concrete smeared cracking);
the brittle cracking model in
Abaqus/Explicit
(Cracking model for concrete);
and the concrete damaged plasticity model in both
Abaqus/Standard
and
Abaqus/Explicit
(Concrete damaged plasticity).
Each model is designed to provide a general capability for modeling plain and
reinforced concrete (as well as other similar quasibrittle materials) in all
types of structures: beams, trusses, shells, and solids.
The smeared crack concrete model in
Abaqus/Standard is
intended for applications in which the concrete is subjected to essentially
monotonic straining and a material point exhibits either tensile cracking or
compressive crushing. Plastic straining in compression is controlled by a
“compression” yield surface. Cracking is assumed to be the most important
aspect of the behavior, and the representation of cracking and postcracking
anisotropic behavior dominates the modeling.
The brittle cracking model in
Abaqus/Explicit
is intended for applications in which the concrete behavior is dominated by
tensile cracking and compressive failure is not important. The model includes
consideration of the anisotropy induced by cracking. In compression, the model
assumes elastic behavior. A simple brittle failure criterion is available to
allow the removal of elements from a mesh.
The concrete damaged plasticity model in
Abaqus/Standard and
Abaqus/Explicit
is based on the assumption of scalar (isotropic) damage and is designed for
applications in which the concrete is subjected to arbitrary loading
conditions, including cyclic loading. The model takes into consideration the
degradation of the elastic stiffness induced by plastic straining both in
tension and compression. It also accounts for stiffness recovery effects under
cyclic loading.
 Progressive damage
and failure

Abaqus/Explicit
offers a general capability for modeling progressive damage and failure in
ductile metals and fiberreinforced composites (Progressive Damage and Failure).
Plasticity theories
Most materials of engineering interest initially respond elastically.
Elastic behavior means that the deformation is fully recoverable: when the load
is removed, the specimen returns to its original shape. If the load exceeds
some limit (the “yield load”), the deformation is no longer fully recoverable.
Some part of the deformation will remain when the load is removed, as, for
example, when a paperclip is bent too much or when a billet of metal is rolled
or forged in a manufacturing process. Plasticity theories model the material's
mechanical response as it undergoes such nonrecoverable deformation in a
ductile fashion. The theories have been developed most intensively for metals,
but they are also applied to soils, concrete, rock, ice, crushable foam, and so
on. These materials behave in very different ways. For example, large values of
pure hydrostatic pressure cause very little inelastic deformation in metals,
but quite small hydrostatic pressure values may cause a significant,
nonrecoverable volume change in a soil sample. Nonetheless, the fundamental
concepts of plasticity theories are sufficiently general that models based on
these concepts have been developed successfully for a wide range of materials.
Most of the plasticity models in
Abaqus
are “incremental” theories in which the mechanical strain rate is decomposed
into an elastic part and a plastic (inelastic) part. Incremental plasticity
models are usually formulated in terms of

a yield surface, which generalizes the
concept of “yield load” into a test function that can be used to determine if
the material responds purely elastically at a particular state of stress,
temperature, etc;

a flow rule, which defines the inelastic
deformation that occurs if the material point is no longer responding purely
elastically; and

evolution laws that define the
hardening—the way in which the yield and/or flow
definitions change as inelastic deformation occurs.
Abaqus/Standard
also has a “deformation” plasticity model, in which the stress is defined from
the total mechanical strain. This is a RambergOsgood model (Deformation plasticity)
and is intended primarily for ductile fracture mechanics applications, where
fully plastic solutions are often required.
Elastic response
The
Abaqus
plasticity models also need an elasticity definition to deal with the
recoverable part of the strain. In
Abaqus
the elasticity is defined by including linear elastic behavior or, if relevant
for some plasticity models, porous elastic behavior in the same material
definition (see
Material data definition).
In the case of the Mises and JohnsonCook plasticity models in
Abaqus/Explicit
the elasticity can alternatively be defined using an equation of state with
associated deviatoric behavior (see
Equation of state).
When performing an elasticplastic analysis at finite strains,
Abaqus
assumes that the plastic strains dominate the deformation and that the elastic
strains are small. This restriction is imposed by the elasticity models that
Abaqus
uses. It is justified because most materials have a welldefined yield point
that is a very small percentage of their Young's modulus; for example, the
yield stress of metals is typically less than 1% of the Young's modulus of the
material. Therefore, the elastic strains will also be less than this
percentage, and the elastic response of the material can be modeled quite
accurately as being linear.
In
Abaqus/Explicit
the elastic strain energy reported is updated incrementally. The incremental
change in elastic strain energy ($\mathrm{\Delta}{E}_{s}$)
is computed as $\mathrm{\Delta}{E}_{s}=\mathrm{\Delta}{E}_{t}\mathrm{\Delta}{E}_{p}$,
where $\mathrm{\Delta}{E}_{t}$
is the incremental change in total strain energy and $\mathrm{\Delta}{E}_{p}$
is the incremental change in plastic energy dissipation.
$\mathrm{\Delta}{E}_{s}$
is much smaller than $\mathrm{\Delta}{E}_{t}$
and $\mathrm{\Delta}{E}_{p}$
for increments in which the deformation is almost all plastic. Approximations
in the calculations of $\mathrm{\Delta}{E}_{t}$
and $\mathrm{\Delta}{E}_{p}$
result in deviations from the true solutions that are insignificant compared to
$\mathrm{\Delta}{E}_{t}$
and $\mathrm{\Delta}{E}_{p}$
but can be significant relative to $\mathrm{\Delta}{E}_{s}$.
Typically, the elastic strain energy solution is quite accurate, but in some
rare cases the approximations in the calculations of $\mathrm{\Delta}{E}_{t}$
and $\mathrm{\Delta}{E}_{p}$
can lead to a negative value reported for the elastic strain energy. These
negative values are most likely to occur in an analysis that uses
ratedependent plasticity. As long as the absolute value of the elastic strain
energy is very small compared to the total strain energy, a negative value for
the elastic strain energy should not be considered an indication of a serious
solution problem.
Stress and strain measures
Most materials that exhibit ductile behavior (large inelastic strains) yield
at stress levels that are orders of magnitude less than the elastic modulus of
the material, which implies that the relevant stress and strain measures are
“true” stress (Cauchy stress) and logarithmic strain. Material data for all of
these models should, therefore, be given in these measures.
If you have nominal stressstrain data for a uniaxial test and the material
is isotropic, a simple conversion to true stress and logarithmic plastic strain
is
$${\sigma}_{\mathrm{true}}={\sigma}_{\mathrm{nom}}\left(1+{\epsilon}_{\mathrm{nom}}\right),$$
$${\epsilon}_{\mathrm{ln}}^{\mathrm{pl}}=\mathrm{ln}\left(1+{\epsilon}_{\mathrm{nom}}\right)\frac{{\sigma}_{\mathrm{true}}}{E},$$
where E is the Young's modulus.
Specifying initial equivalent plastic strains
Initial values of equivalent plastic strain can be specified in
Abaqus
for elements that use classical metal plasticity (Classical metal plasticity)
or DruckerPrager plasticity (Extended DruckerPrager models)
by defining initial hardening conditions (Initial conditions in Abaqus/Standard and Abaqus/Explicit).
The equivalent plastic strain (output variable PEEQ) then contains the initial value of equivalent plastic strain
plus any additional equivalent plastic strain due to plastic straining during
the analysis. However, the plastic strain tensor (output variable PE) contains only the amount of straining due to deformation
during the analysis.
The simple onedimensional example shown in
Figure 2
illustrates the concept.
Figure 2. Initial equivalent plastic strain example.
The material is in an annealed configuration at point
A; its yield stress is ${\sigma}_{B}^{0}$.
It is then hardened by loading it along the path $\left(A,B,C,D\right)$;
the new yield stress is ${\sigma}_{E}^{0}$.
A new analysis that employs the same hardening curve as the first analysis
takes this material along the path $\left(D,E,F\right)$,
starting from point D, by specifying a total strain,
${\epsilon}_{2}$.
Plastic strain ${\epsilon}_{2}^{pl}$
will result and can be output (for instance) using output variable PE11. To obtain the correct yield stress, ${\sigma}_{E}^{0}$,
the equivalent plastic strain at point E,
${\epsilon}_{1}^{pl}$,
should be provided as an initial condition. Likewise, the correct yield stress
at point F is obtained from an equivalent plastic strain PEEQ$={\epsilon}_{1}^{pl}+{\epsilon}_{2}^{pl}$.
