You can typically use the classical metal plasticity models (Classical Metal Plasticity) to describe the
yield and inelastic flow of a metal at relatively low temperatures, where loading is
relatively monotonic and creep effects are not important. In Abaqus these models use standard Mises or quadratic 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
You can use a linear kinematic hardening model or a nonlinear isotropic/kinematic
hardening model (Models for Metals Subjected to Cyclic Loading) 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).
You can simulate the Bauschinger effect and plastic shakedown with both models, but
the nonlinear isotropic/kinematic hardening model provides more accurate predictions.
Ratcheting and relaxation of the mean stress are accounted for only by the nonlinear
isotropic/kinematic model. In addition to these two models, you can use the
ORNL model in Abaqus/Standard if you require a simple life estimation for the design of stainless steels subjected
to low-cycle fatigue and creep fatigue (see below).
Rate-dependent yield
As strain rates increase, many materials show an increase in their yield strength. You
can define rate dependence (Rate-Dependent Yield) in Abaqus for a number of plasticity models. Rate dependence is available in both static and
dynamic procedures. Applicable models include classical metal plasticity, extended
Drucker-Prager plasticity, and crushable foam plasticity.
Creep and swelling
Abaqus/Standard provides a material model for classical metal creep behavior and time-dependent
volumetric swelling behavior (Rate-Dependent Plasticity: Creep and Swelling). This model is
intended for relatively slow (quasi-static) inelastic deformation of a model such as the
high-temperature 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. You can use creep with the classical metal
plasticity model, with the ORNL model, and to define
rate-dependent gasket behavior (Defining the Gasket Behavior Directly Using a Gasket Behavior Model). Swelling
is available with the classical metal plasticity model. (Usage with the Drucker-Prager
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 user-defined temperature, known as the annealing
temperature (Annealing or Melting). It is intended for use with
metals subjected to high-temperature deformation processes, in which the material might
undergo melting and possibly resolidification or some other form of annealing. In Abaqus, you can model annealing or melting with classical metal plasticity (Mises and
Hill); in Abaqus/Explicit, you can also model annealing or melting with Johnson-Cook 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.
Hill anisotropic yield and creep
Abaqus provides an anisotropic yield model using Hill's quadratic potential (Hill 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 creep (Rate-Dependent 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 because of loading.
Nonquadratic yield
Abaqus provides yield models using nonquadratic stress potential functions (Nonquadratic Yield), such as Tresca
and Hosford yield surfaces for isotropic yield and Barlat yield surfaces for anisotropic
yield. Compared with Hill anisotropic plasticity, Barlat anisotropic plasticity provides
flexibility for describing more complex anisotropic yield behavior. Abaqus uses the anisotropy coefficients specified for Barlat yield surfaces to define the
initial anisotropy. The model is not adequate for cases in which the anisotropy changes
significantly as the material deforms because of loading.
Johnson-Cook plasticity
The Johnson-Cook plasticity model in Abaqus/Explicit (Johnson-Cook Plasticity) is particularly suited to model
high-strain-rate 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 available in Abaqus/Explicit for the Mises and Johnson-Cook plasticity models (Dynamic Failure Models):
the shear failure model, where the failure criterion is based on the accumulated
equivalent plastic strain,
and 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
quasi-static and dynamic situations and have other significant advantages.
Porous metal plasticity
The porous metal plasticity model (Porous Metal Plasticity) models
materials that exhibit damage in the form of void initiation and growth. You can also
use it 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.
Two-layer viscoplasticity
The two-layer viscoplasticity model in Abaqus/Standard (Two-Layer Viscoplasticity) is useful for modeling materials in which
significant time-dependent behavior and plasticity occur. For metals this behavior
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
high-temperature creep of type 304 and 316 stainless steel. Plasticity and creep
calculations are provided according to the specification in Nuclear Standard
NEF 9-5T, “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 low-cycle fatigue and creep fatigue are
critical issues.
Deformation plasticity
Abaqus/Standard provides a deformation theory Ramberg-Osgood 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 small-displacement analysis for which the fully plastic
solution must be developed in a part of the model.
Extended Drucker-Prager plasticity and creep
The extended Drucker-Prager family of plasticity models (Extended Drucker-Prager Models) describes the behavior of granular materials or
polymers in which the yield behavior depends on the equivalent pressure stress. The
inelastic deformation can 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 time-dependent (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 Drucker-Prager/Cap plasticity and creep
The modified Drucker-Prager/Cap plasticity model (Modified Drucker-Prager/Cap Model) can be used to simulate geological materials that exhibit pressure-dependent 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 time-dependent (creep) behavior coupled with the plastic behavior is also
available for this model, with two possible creep mechanisms are possible: a cohesion,
Drucker-Prager−like mechanism; and a consolidation, cap-like mechanism.
Mohr-Coulomb plasticity
The Mohr-Coulomb plasticity model (Mohr-Coulomb Plasticity) can be
used for design applications in the geotechnical engineering area. The model uses the
classical Mohr-Coloumb yield criterion: a straight line in the meridional plane and an
irregular hexagonal section in the deviatoric plane. However, the Abaqus Mohr-Coulomb 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 available 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
quasi-brittle 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 fiber-reinforced 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 remains when the
load is removed; 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 other materials. 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 can
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 has a purely
elastic response at a particular state of stress, temperature, and other values;
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 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 Ramberg-Osgood 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 Johnson-Cook 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 elastic-plastic 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 well-defined 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 () is computed as , where is the incremental change in total strain energy and is the incremental change in plastic energy dissipation. is much smaller than and for increments in which the deformation is almost all plastic.
Approximations in the calculations of and result in deviations from the true solutions that are insignificant
compared to and but can be significant relative to . Typically, the elastic strain energy solution is quite accurate, but in
some rare cases the approximations in the calculations of and 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 rate-dependent plasticity.
If 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 stress-strain data for a uniaxial test and the material is isotropic, a
simple conversion to true stress and logarithmic plastic strain is
where E is the Young's modulus.
Example of Stress-Strain Data Input
The example below illustrates the input of material data for the classical metal
plasticity model with isotropic hardening (Classical Metal Plasticity).
Stress-strain data representing the material hardening behavior are necessary to define
the model. An experimental hardening curve might appear as that shown in Figure 1.
Figure 1. Experimental hardening curve.
First yield occurs at 200 MPa (29000 lb/in2). The material then hardens to 300
MPa (43511 lb/in2) at one percent strain, after which it is perfectly plastic.
Assuming that the Young's modulus is 200000 MPa (29 × 106 lb/in2),
the plastic strain at the one percent strain point is .01 − 300/200000=.0085. When the
units are newtons and millimeters, the input is
Yield Stress
Plastic Strain
200.
0.
300.
.0085
Plastic strain values, not total strain values, are used in defining the hardening
behavior. Furthermore, the first data pair must correspond with the onset of plasticity
(the plastic strain value must be zero in the first pair). These concepts are applicable
when hardening data are defined in a tabular form for any of the following plasticity
models:
The input required to define hardening is discussed in the referenced sections.
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 Drucker-Prager plasticity (Extended Drucker-Prager Models) by defining initial hardening conditions (Initial Conditions). The
equivalent plastic strain (output variable
PEEQ) then contains the initial value of
equivalent plastic strain plus any additional equivalent plastic strain because of 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 one-dimensional example shown in Figure 2 illustrates the concept.
The material is in an annealed configuration at point A; its yield
stress is . It is then hardened by loading it along the path ; the new yield stress is . A new analysis that uses the same hardening curve as the first analysis
takes this material along the path , starting from point D, by specifying a total
strain, . Plastic strain will result and can be output (for example) using output variable
PE11. To obtain the correct yield
stress, , the equivalent plastic strain at point E, , should be provided as an initial condition. Likewise, the correct yield
stress at point F is obtained from an equivalent plastic strain PEEQ.