The classical deviatoric metal creep behavior in Abaqus/Standard:
can be defined using user subroutine CREEP or by providing parameters as
input for some simple creep laws;
can model either isotropic creep (using Mises stress potential) or anisotropic creep
(using Hill's anisotropic stress potential);
is active only during steps using the coupled temperature-displacement procedure, the
transient soils consolidation procedure, and the quasi-static procedure;
requires that the material's elasticity be defined as linear elastic behavior;
can be modified to implement the auxiliary creep hardening rules specified in Nuclear
Standard NEF 9-5T, “Guidelines and Procedures for Design
of Class 1 Elevated Temperature Nuclear System Components”; these rules are exercised by
means of a constitutive model developed by Oak Ridge National Laboratory (ORNL – Oak Ridge National Laboratory Constitutive Model);
can be used in combination with creep strain rate control in analyses in which the creep
strain rate must be kept within a certain range; and
can potentially result in errors in calculated creep strains if anisotropic creep and
plasticity occur simultaneously (discussed below).
Rate-dependent gasket behavior in Abaqus/Standard:
uses unidirectional creep as part of the model of the gasket's thickness-direction
behavior;
can be defined using user subroutine CREEP or by providing parameters as
input for some simple creep laws;
is active only during steps using the quasi-static procedure; and
requires that an elastic-plastic model be used to define the rate-independent part of the
thickness-direction behavior of the gasket.
Volumetric swelling behavior in Abaqus/Standard:
can be defined using user subroutine CREEP or by providing tabular input;
can be either isotropic or anisotropic;
is active only during steps using the coupled temperature-displacement procedure, the
transient soils consolidation procedure, and the quasi-static procedure; and
requires that the material's elasticity be defined as linear elastic behavior.
Creep behavior is specified by the equivalent uniaxial behavior—the creep “law.” In
practical cases, creep laws are typically of very complex form to fit experimental data;
therefore, the laws are defined with user subroutine CREEP, as discussed below.
Alternatively, five common creep laws are provided in Abaqus/Standard: the power law, the hyperbolic-sine law, the double power law, the Anand law, and the
Darveaux law. These standard creep laws are used for modeling secondary or steady-state
creep. Creep is defined by including creep behavior in the material model definition (Material Data Definition). Alternatively, creep can be defined in conjunction
with gasket behavior to define the rate-dependent behavior of a gasket.
Input File Usage
Use the following options to include creep behavior in the material model
definition:
Property module: material editor: MechanicalPlasticityCreep
Choosing a Creep Model
The power law creep model is attractive for its simplicity. However, it is limited in its
range of application. The time-hardening version of the power law creep model is typically
recommended only in cases when the stress state remains essentially constant. The
strain-hardening version of power law creep should be used when the stress state varies
during an analysis. In the case where the stress is constant and there are no temperature
or field dependencies, the time-hardening and strain-hardening versions of the power creep
law are equivalent. For either version of the power law, the stresses should be relatively
low.
In regions of high stress, such as around a crack tip, the creep strain rates frequently
show an exponential dependence of stress. The hyperbolic-sine creep law shows exponential
dependence on the stress, , at high stress levels (, where is the yield stress) and reduces to the power law at low stress levels
(with no explicit time dependence).
The double power, Anand, and Darveaux models are particularly well suited for modeling
the behavior of solder alloys used in electronic packaging and have been shown to produce
accurate results for a wide range of temperatures and strain rates.
None of the above models is suitable for modeling creep under cyclic loading. The
ORNL model (ORNL – Oak Ridge National Laboratory Constitutive Model) is an
empirical model for stainless steel that gives approximate results for cyclic loading
without having to perform the cyclic loading numerically. Generally, creep models for
cyclic loading are complicated and must be added to a model with user subroutine CREEP or with user subroutine UMAT.
Modeling Simultaneous Creep and Plasticity
If creep and plasticity occur simultaneously and implicit creep integration is in effect,
both behaviors might interact and a coupled system of constitutive equations needs to be
solved. If creep and plasticity are isotropic, Abaqus/Standard properly takes into account such coupled behavior, even if the elasticity is
anisotropic. However, if either creep or plasticity are anisotropic, Abaqus/Standard integrates the creep equations without taking plasticity into account, which might lead
to substantial errors in the creep strains. This situation develops only if plasticity and
creep are active at the same time, such as would occur during a long-term load increase;
you would not expect to have a problem if there is a short-term preloading phase in which
plasticity dominates, followed by a creeping phase in which no further yielding occurs.
Integration of the creep laws and rate-dependent plasticity are discussed in Rate-dependent metal plasticity (creep).
Time Power Law and Power Law Models
The time power law and power law models described below are equivalent to the “time
hardening” and the “strain hardening” forms but avoid their drawbacks. The time power law
and power law models rewrite the laws in such a way that the typical parameter values do
not cause numerical difficulties. In addition, the units of all the parameters are
physical, which makes unit conversion easier if it is required.
Time Power Law Model
The time power law model has the following form:
where is Mises equivalent stress or Hill's anisotropic equivalent deviatoric
stress according to whether isotropic or anisotropic creep behavior is defined and , , , and are material parameters.
The model is equivalent to the time hardening form. It is recommended
that you use the time power law model when the value of the parameter is very small (). In this case the equivalent time power law model is obtained by
setting , keeping the parameters and unchanged, and setting to an arbitrary value greater than zero (typically, is set to one).
Property module: material editor: MechanicalPlasticityCreep: Law: Time Power
Power Law Model
The power law model has the following form:
where
is the uniaxial equivalent creep strain rate,
is the equivalent creep strain,
is the uniaxial equivalent deviatoric stress, and
are material parameters.
This model is equivalent to the strain hardening form. It is recommended
that you use the power law model when the value of the parameter is very small (). In this case the equivalent power law model is obtained by setting , keeping the parameters and unchanged, and setting to an arbitrary value greater than zero (typically, is set to one).
Property module: material editor: MechanicalPlasticityCreep: Law: Power
Time/Strain Hardening Models
Time hardening and strain hardening models to specify creep are available. However, to
avoid the drawbacks of these models, it is recommended that you use the time power law and
power law models (see Time Power Law and Power Law Models).
Time Hardening Form
The “time hardening” form is the simpler of the two forms and is defined as
where
is the uniaxial equivalent creep strain rate,
is the uniaxial equivalent deviatoric stress,
t
is the total or the creep time, and
A, n, and
m
are defined by you as functions of temperature.
For physically reasonable behavior A and
n must be positive and .
Property module: material editor: MechanicalPlasticityCreep: Law: Strain-Hardening
Numerical Difficulties
Depending on the choice of units for either form, the value of A
might be very small for typical creep strain rates. If A is less
than 10−27, numerical difficulties can cause errors in the material
calculations. Therefore, use another system of units or use the time power law or power
law model (described below) to avoid such difficulties in the calculation of creep
strain increments.
Time-Dependent Behavior
In the time hardening form and the time power law model, the total time or
the creep time can be used. The total time is the accumulated time over all general
analysis steps. The creep time is the sum of the times of the procedures with
time-dependent material behavior. If the total time is used, it is recommended that small
step times compared to the creep time be used for any steps for which creep is not active
in an analysis; this is necessary to avoid changes in hardening behavior in subsequent
steps.
Property module: material editor: MechanicalPlasticityCreep: Time: Total or Creep
Hyperbolic-Sine Law Model
The hyperbolic-sine law is available in the form
where
and
are defined above,
is the temperature,
is the user-defined value of absolute zero on the temperature scale used,
is the activation energy,
R
is the universal gas constant, and
A, B, and
n
are other material parameters.
This model includes temperature dependence, which is apparent in the above expression;
however, the parameters A, B,
n, , and R cannot be defined as functions of
temperature.
Property module: material editor: MechanicalPlasticityCreep: Law: Hyperbolic-Sine
Any module: ModelEdit Attributesmodel_name: Absolute zero temperature
Numerical Difficulties
As with the power law, A might be very small for typical creep
strain rates. If A is very small (such as less than
10−27), use another system of units to avoid numerical difficulties in the
calculation of creep strain increments.
Anand Model
The Anand model is available in the form
where
, , R, , and
are defined above,
is the activation energy,
is the deformation resistance, and
, , and
are material parameters.
The evolution equation for the deformation resistance, (initially ), is
with
where
and , , , , , , , and are material parameters.
In addition, the initial deformation resistance is a function of temperature of the form
Property module: material editor: MechanicalPlasticityCreep: Law: Anand
Any module: ModelEdit Attributesmodel_name: Absolute zero temperature
Darveaux Model
The Darveau model involves both primary and secondary creep. The secondary creep
(steady-state) component is described by a standard hyperbolic sine law
The steady-state law is modified to include the primary creep effects through
where
, , R, Q, , and
are defined above,
is the steady-state creep prefactor,
is the steady-state creep power law breakdown, and
Property module: material editor: MechanicalPlasticityCreep: Law: Double Power
Any module: ModelEdit Attributesmodel_name: Absolute zero temperature
Anisotropic Creep
Anisotropic creep can be defined to specify the stress ratios that appear in Hill's
function. You must define the ratios in each direction that will be used to scale the stress value when the
creep strain rate is calculated. The ratios can be defined as constant or dependent on
temperature and other predefined field variables. The ratios are defined with respect to
the user-defined local material directions or the default directions (see Orientations). Further
details are provided in Hill Anisotropic Yield/Creep. Anisotropic creep is not
available when creep is used to define a rate-dependent gasket behavior since only the
gasket thickness-direction behavior can have rate-dependent behavior.
Property module: material editor: MechanicalPlasticityCreep: SuboptionsPotential
Volumetric Swelling Behavior
As with the creep laws, volumetric swelling laws are usually complex and are most
conveniently specified in user subroutine CREEP as discussed below. However, a
means of tabular input is also provided for the form
where is the volumetric strain rate caused by swelling and , , are predefined fields such as irradiation fluxes in cases involving
nuclear radiation effects. Up to six predefined fields can be specified.
Volumetric swelling cannot be used to define a rate-dependent gasket behavior.
Property module: material editor: MechanicalPlasticitySwelling
Anisotropic Swelling
Anisotropy can easily be included in the swelling behavior. If anisotropic swelling
behavior is defined, the anisotropic swelling strain rate is expressed as
where is the volumetric swelling strain rate that you define either directly
(discussed above) or in user subroutine CREEP. The ratios , , and are also user-defined. The directions of the components of the swelling
strain rate are defined by the local material directions, which can be either user-defined
or the default directions (see Orientations).
Property module: material editor: MechanicalPlasticitySwelling: SuboptionsRatios
User Subroutine CREEP
User subroutine CREEP provides a very general
capability for implementing viscoplastic models such as creep and swelling models in which
the strain rate potential can be written as a function of equivalent pressure stress,
p; the Mises or Hill's equivalent deviatoric stress, ; and any number of solution-dependent state variables. Solution-dependent
state variables are used in conjunction with the constitutive definition; their values
evolve with the solution and can be defined in this subroutine. Examples are hardening
variables associated with the model.
The user subroutine can also be used to define very general rate- and time-dependent
thickness-direction gasket behavior. When an even more general form is required for the
strain rate potential, user subroutine UMAT (User-Defined Mechanical Material Behavior) can be used.
Input File Usage
Use one or both of the following options. Only the first option can be used to define
gasket behavior.
Use one or both of the following models. Only the first model can be used to define
gasket behavior.
Property module: material editor:
MechanicalPlasticityCreep: Law: User definedMechanicalPlasticitySwelling: Law: User subroutine CREEP
Removing Creep Effects in an Analysis Step
You can specify that no creep (or viscoelastic) response can occur during certain analysis
steps, even if creep (or viscoelastic) material properties have been defined.
Step module: Create Step:
Coupled temp-displacement: toggle off Include creep/swelling/viscoelastic behavior
Soils: Pore fluid response: Transient consolidation: toggle off Include creep/swelling/viscoelastic behavior
Integration
Explicit integration, implicit integration, or both integration schemes can be used in a
creep analysis, depending on the procedure used, the parameters specified for the procedure,
the presence of plasticity, and whether or not geometric nonlinearity is requested.
Application of Explicit and Implicit Schemes
Nonlinear creep problems are often solved efficiently by forward-difference integration
of the inelastic strains (the “initial strain” method). This explicit method is
computationally efficient because, unlike implicit methods, iteration is not required.
Although this method is only conditionally stable, the numerical stability limit of the
explicit operator is usually sufficiently large to allow the solution to be developed in a
small number of time increments.
Abaqus/Standard uses either an explicit or an implicit integration scheme or switches from explicit to
implicit in the same step. These schemes are outlined first, followed by a description of
which procedures use these integration schemes.
Integration scheme 1: Starts with explicit integration and switches to implicit
integration based on either stability or if plasticity is active. The stability limit
used in explicit integration is discussed in the next section.
Integration scheme 2: Starts with explicit integration and switches to implicit
integration when plasticity is active. The stability criterion does not play a role
here.
The use of the above integration schemes is determined by the procedure type, your choice
of the integration type to be used, as well as whether or not geometric nonlinearity is
requested. For quasi-static and coupled temperature-displacement procedures, if you do not
choose an integration type, integration scheme 1 is used for a geometrically linear
analysis and integration scheme 3 is used for a geometrically nonlinear analysis. You can
force Abaqus/Standard to use explicit integration for creep and swelling effects in coupled
temperature-displacement or quasi-static procedures, when plasticity is not active
throughout the step (integration scheme 2). Explicit integration can be used regardless of
whether or not geometric nonlinearity has been requested (see General and Perturbation Procedures).
For a transient soils consolidation procedure, the implicit integration scheme
(integration scheme 3) is always used, irrespective of whether a geometrically linear or
nonlinear analysis is performed.
Input File Usage
Use one of the following options to restrict Abaqus/Standard to using explicit integration:
Coupled temp-displacement: toggle on Include creep/swelling/viscoelastic behavior: Incrementation: Creep/swelling/viscoelastic integration: Explicit
Automatic Monitoring of Stability Limit during Explicit Integration
Abaqus/Standard monitors the stability limit automatically during explicit integration. If, at any
point in the model, the creep strain increment is larger than the total elastic strain, the problem will become
unstable. Therefore, a stable time step, , is calculated every increment by
where is the equivalent total elastic strain at time t,
the beginning of the increment, and is the equivalent creep strain rate at time t.
Furthermore,
where is the Mises stress at time t, and
where
is the gradient of the deviatoric stress potential,
is the elasticity matrix, and
is an effective elastic modulus—for isotropic elasticity can be approximated by Young's modulus.
At every increment for which explicit integration is performed, the stable time
increment, , is compared to the critical time increment, , which is calculated as follows:
The quantity errtol is an error tolerance that you define as
discussed below. If is less than , is used as the time increment, which would mean that the stability
criterion was limiting the size of the time step further than required by accuracy
considerations. Abaqus/Standard will automatically switch to the backward difference operator (the implicit method,
which is unconditionally stable) if is less than for nine consecutive increments, you have not restricted Abaqus/Standard to explicit integration as discussed above, and there is sufficient time left in the
analysis (time left ). The stiffness matrix will be reformed at every iteration if the
implicit algorithm is used.
Specifying the Tolerance for Automatic Incrementation
The integration tolerance must be chosen so that increments in stress, , are calculated accurately. Consider a one-dimensional example. The
stress increment, , is
where , , and are the uniaxial elastic, total, and creep strain increments,
respectively, and E is the elastic modulus. For to be calculated accurately, the error in the creep strain increment, , must be small compared to ; that is,
Measuring the error in as
leads to
You define errtol for the applicable procedure by choosing an
acceptable stress error tolerance and dividing this by a typical elastic modulus;
therefore, it should be a small fraction of the ratio of the typical stress and the
effective elastic modulus in a problem. It is important to recognize that this approach
for selecting a value for errtol is often very conservative,
and acceptable solutions can usually be obtained with higher values.
Step module: Create Step:
Visco: Incrementation: toggle on Creep/swelling/viscoelastic strain errortolerance, and enter a value
Coupled temp-displacement: toggle on Include creep/swelling/viscoelastic behavior: Incrementation: toggle on Creep/swelling/viscoelastic strain error tolerance, and enter a value
Soils: Pore fluid response: Transient consolidation: toggle on Include creep/swelling/viscoelastic behavior: Incrementation: toggle on Creep/swelling/viscoelastic strain error tolerance, and enter a value
Loading Control Using Creep Strain Rate
In superplastic forming a controllable pressure is applied to deform a body. Superplastic
materials can deform to very large strains, provided that the strain rates of the
deformation are maintained within very tight tolerances. The objective of the superplastic
analysis is to predict how the pressure must be controlled to form the component as fast as
possible without exceeding a superplastic strain rate anywhere in the material.
To achieve this using Abaqus/Standard, the controlling algorithm is as follows. During an increment Abaqus/Standard calculates , the maximum value of the ratio of the equivalent creep strain rate to the
target creep strain rate for any integration point in a specified element set. If is less than 0.2 or greater than 3.0 in a given increment, the increment
is abandoned and restarted with the following load modifications:
where p is the new load magnitude and is the old load magnitude. If , the increment is accepted; and at the beginning of the following time
increment, the load magnitudes are modified as follows:
When you activate the above algorithm, the loading in a creep and/or swelling problem can
be controlled on the basis of the maximum equivalent creep strain rate found in a defined
element set. As a minimum requirement, this method is used to define a target equivalent
creep strain rate; however, if required, it can also be used to define the target creep
strain rate as a function of equivalent creep strain (measured as log strain), temperature,
and other predefined field variables. The creep strain dependency curve at each temperature
must always start at zero equivalent creep strain.
The AMPLITUDE option must appear in the
model definition portion of an input file, while the loading options (CLOAD, DLOAD, DSLOAD, and BOUNDARY) and the CREEP STRAIN RATE CONTROL option
should appear in each relevant step definition.
Abaqus/CAE Usage
Creep strain rate control is not supported in Abaqus/CAE.
Elements
Rate-dependent plasticity (creep and swelling behavior) can be used with any continuum,
shell, membrane, gasket, and beam element in Abaqus/Standard that has displacement degrees of freedom. Creep (but not swelling) can also be defined in
the thickness direction of any gasket element in conjunction with the gasket behavior
definition.
Output
In addition to the standard output identifiers available in Abaqus/Standard (Abaqus/Standard Output Variable Identifiers), the following
variables relate directly to creep and swelling models:
CEEQ
Equivalent creep strain, .
CESW
Magnitude of swelling strain.
SDEFRES
Deformation resistance, . This output is relevant only for the Anand model.
The following output, which is relevant only for an analysis with creep strain rate loading
control as discussed above, is printed at the beginning of an increment and is written
automatically to the results file and output database file when any output to these files is
requested:
RATIO
Maximum value of the ratio of the equivalent creep strain rate to the target creep
strain rate, .
AMPCU
Current value of the solution-dependent amplitude.