ProductsAbaqus/StandardAbaqus/CAE Creep behaviorCreep 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 hyperbolicsine law, the double power law, the Anand law, and the Darveaux law. These standard creep laws are used for modeling secondary or steadystate 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 ratedependent behavior of a gasket. Input File Usage Use the following options to include creep behavior in the material model definition: MATERIAL CREEP Use the following options to define creep in conjunction with gasket behavior: GASKET BEHAVIOR CREEP Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityCreep
Choosing a creep modelThe powerlaw creep model is attractive for its simplicity. However, it is limited in its range of application. The timehardening version of the powerlaw creep model is typically recommended only in cases when the stress state remains essentially constant. The strainhardening version of powerlaw 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 and/or field dependencies, the timehardening and strainhardening versions of the powercreep 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 hyperbolicsine creep law shows exponential dependence on the stress, $\sigma $, at high stress levels ($\sigma /{\sigma}^{0}\gg 1$, where ${\sigma}^{0}$ is the yield stress) and reduces to the powerlaw 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 plasticityIf creep and plasticity occur simultaneously and implicit creep integration is in effect, both behaviors may 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 creep and plasticity are anisotropic, Abaqus/Standard integrates the creep equations without taking plasticity into account, which may 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 longterm load increase; one would not expect to have a problem if there is a shortterm preloading phase in which plasticity dominates, followed by a creeping phase in which no further yielding occurs. Integration of the creep laws and ratedependent plasticity are discussed in Ratedependent metal plasticity (creep). Powerlaw modelThe powerlaw model can be used in its “time hardening” form or in the corresponding “strain hardening” form. Time hardening formThe “time hardening” form is the simpler of the two forms of the powerlaw model: $${\dot{\overline{\epsilon}}}^{cr}=A{\stackrel{~}{q}}^{n}{t}^{m},$$
where
$\stackrel{~}{q}$ is Mises equivalent stress or Hill's anisotropic equivalent deviatoric stress according to whether isotropic or anisotropic creep behavior is defined (discussed below). For physically reasonable behavior A and n must be positive and $1<m\le 0$. Input File Usage CREEP, LAW=TIME Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityCreep: Law: TimeHardening Timedependent behaviorIn the time hardening 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 timedependent 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. Abaqus/CAE Usage Specifying the time type is not supported in Abaqus/CAE. Strain hardening formThe “strain hardening” form of the power law is $${\dot{\overline{\epsilon}}}^{cr}={\left(A{\stackrel{~}{q}}^{n}{\left[\left(m+1\right){\overline{\epsilon}}^{cr}\right]}^{m}\right)}^{\frac{1}{m+1}},$$
where ${\dot{\overline{\epsilon}}}^{cr}$ and $\stackrel{~}{q}$ are defined above and ${\overline{\epsilon}}^{cr}$ is the equivalent creep strain. Input File Usage CREEP, LAW=STRAIN Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityCreep: Law: StrainHardening Numerical difficultiesDepending on the choice of units for either form of the power law, the value of A may 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 to avoid such difficulties in the calculation of creep strain increments. Hyperbolicsine law modelThe hyperbolicsine law is available in the form $${\dot{\overline{\epsilon}}}^{cr}=A{\left(\mathrm{sinh}B\stackrel{~}{q}\right)}^{n}\mathrm{exp}\left(\frac{\mathrm{\u25b3}H}{R\left(\theta {\theta}^{Z}\right)}\right),$$
where
This model includes temperature dependence, which is apparent in the above expression; however, the parameters A, B, n, $\mathrm{\u25b3}H$, and R cannot be defined as functions of temperature. Input File Usage Use both of the following options: CREEP, LAW=HYPERB PHYSICAL CONSTANTS, ABSOLUTE ZERO=${\theta}^{Z}$ Abaqus/CAE Usage Define both of the following: Property module: material editor: MechanicalPlasticityCreep: Law: HyperbolicSine Any module: ModelEdit Attributesmodel_name: Absolute zero temperature Numerical difficultiesAs with the power law, A may 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 modelThe Anand model is available in the form $${\dot{\overline{\epsilon}}}^{cr}=A{\left[\mathrm{sinh}\left(\xi \frac{\stackrel{~}{q}}{s}\right)\right]}^{\frac{1}{m}}\mathrm{exp}\left(\frac{Q}{R\left(\theta {\theta}^{Z}\right)}\right),$$
where
The evolution equation for the deformation resistance, $s$ (initially $s={s}_{0}$), is $$\dot{s}={h}_{0}{\left1\frac{s}{{s}^{*}}\right}^{a}sign\left(1\frac{s}{{s}^{*}}\right){\dot{\overline{\epsilon}}}^{cr},$$
with $${s}^{*}=\widehat{s}{\left[\frac{1}{A}{\dot{\overline{\epsilon}}}^{cr}\mathrm{exp}\left(\frac{Q}{R\left(\theta {\theta}^{Z}\right)}\right)\right]}^{n},$$
where $${h}_{0}={A}_{0}+{A}_{1}\left(\theta {\theta}^{Z}\right)+{A}_{2}{\left(\theta {\theta}^{Z}\right)}^{2}+{A}_{3}{\dot{\overline{\epsilon}}}^{cr}+{A}_{4}{\left({\dot{\overline{\epsilon}}}^{cr}\right)}^{2},$$
and $a$, $n$, $\widehat{s}$, ${A}_{0}$, ${A}_{1}$, ${A}_{2}$, ${A}_{3}$, and ${A}_{4}$ are material parameters. In addition, the initial deformation resistance is a function of temperature of the form $${s}_{0}={S}_{1}+{S}_{2}\left(\theta {\theta}^{Z}\right)+{S}_{3}{\left(\theta {\theta}^{Z}\right)}^{2},$$
where ${S}_{1}$, ${S}_{2}$, and ${S}_{3}$ are material parameters. Input File Usage Use both of the following options: CREEP, LAW=ANAND PHYSICAL CONSTANTS, ABSOLUTE ZERO=${\theta}^{Z}$ Abaqus/CAE Usage Specifying the Anand law is not supported in Abaqus/CAE. Darveaux modelThe Darveau model involves both primary and secondary creep. The secondary creep (steadystate) component is described by a standard hyperbolic sine law $${\dot{\overline{\epsilon}}}_{s}^{cr}={C}_{ss}{\left[\mathrm{sinh}\left(\alpha \stackrel{~}{q}\right)\right]}^{n}\mathrm{exp}\left(\frac{Q}{R\left(\theta {\theta}^{Z}\right)}\right).$$
The steadystate law is modified to include the primary creep effects through $${\dot{\overline{\epsilon}}}^{cr}={\dot{\overline{\epsilon}}}_{s}^{cr}[1+{\u03f5}_{T}B\mathrm{exp}(B{\dot{\overline{\epsilon}}}_{s}^{cr}t)],$$
where
Input File Usage Use both of the following options: CREEP, LAW=DARVEAUX PHYSICAL CONSTANTS, ABSOLUTE ZERO=${\theta}^{Z}$ Abaqus/CAE Usage Specifying the Darveaux law is not supported in Abaqus/CAE. Double power modelThe double power law is available in the form $${\dot{\overline{\epsilon}}}^{cr}={A}_{1}\mathrm{exp}\left(\frac{{B}_{1}}{\left(\theta {\theta}^{Z}\right)}\right){\left(\frac{\stackrel{~}{q}}{{\sigma}_{0}}\right)}^{{C}_{1}}+{A}_{2}\mathrm{exp}\left(\frac{{B}_{2}}{\left(\theta {\theta}^{Z}\right)}\right){\left(\frac{\stackrel{~}{q}}{{\sigma}_{0}}\right)}^{{C}_{2}},$$
where
Input File Usage Use both of the following options: CREEP, LAW=DOUBLE POWER PHYSICAL CONSTANTS, ABSOLUTE ZERO=${\theta}^{Z}$ Abaqus/CAE Usage Specifying the double power law is not supported in Abaqus/CAE. Anisotropic creepAnisotropic creep can be defined to specify the stress ratios that appear in Hill's function. You must define the ratios ${R}_{ij}$ 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 userdefined local material directions or the default directions (see Orientations). Further details are provided in Anisotropic yield/creep. Anisotropic creep is not available when creep is used to define a ratedependent gasket behavior since only the gasket thicknessdirection behavior can have ratedependent behavior. Input File Usage POTENTIAL Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityCreep: SuboptionsPotential Volumetric swelling behaviorAs 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 $${\dot{\overline{\epsilon}}}^{sw}=f\left(\theta ,{f}_{1},{f}_{2},\mathrm{\dots}\right),$$
where ${\dot{\overline{\epsilon}}}^{sw}$ is the volumetric strain rate caused by swelling and ${f}_{1}$, ${f}_{2}$, $\mathrm{\dots}$ 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 ratedependent gasket behavior. Input File Usage SWELLING Abaqus/CAE Usage Property module: material editor: MechanicalPlasticitySwelling
Anisotropic swellingAnisotropy can easily be included in the swelling behavior. If anisotropic swelling behavior is defined, the anisotropic swelling strain rate is expressed as $${\dot{\overline{\epsilon}}}_{A}^{sw}={\dot{\overline{\epsilon}}}_{11}^{sw}+{\dot{\overline{\epsilon}}}_{22}^{sw}+{\dot{\overline{\epsilon}}}_{33}^{sw}=\left({r}_{11}+{r}_{22}+{r}_{33}\right)\frac{1}{3}{\dot{\overline{\epsilon}}}^{sw},$$
where ${\dot{\overline{\epsilon}}}^{sw}$ is the volumetric swelling strain rate that you define either directly (discussed above) or in user subroutine CREEP. The ratios ${r}_{11}$, ${r}_{22}$, and ${r}_{33}$ are also userdefined. The directions of the components of the swelling strain rate are defined by the local material directions, which can be either userdefined or the default directions (see Orientations). Abaqus/CAE Usage Property module: material editor: MechanicalPlasticitySwelling: SuboptionsRatios User subroutine CREEPUser 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, $\stackrel{~}{q}$; and any number of solutiondependent state variables. Solutiondependent 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 timedependent thicknessdirection gasket behavior. When an even more general form is required for the strain rate potential, user subroutine UMAT (Userdefined 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. CREEP, LAW=USER SWELLING, LAW=USER Abaqus/CAE Usage 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 defined MechanicalPlasticitySwelling: Law: User subroutine CREEP Removing creep effects in an analysis stepYou can specify that no creep (or viscoelastic) response can occur during certain analysis steps, even if creep (or viscoelastic) material properties have been defined. Input File Usage Use one of the following options: COUPLED TEMPERATUREDISPLACEMENT, CREEP=NONE SOILS, CONSOLIDATION, CREEP=NONE Abaqus/CAE Usage Use one of the following options: Step module: Create Step: Coupled tempdisplacement: toggle off Include creep/swelling/ viscoelastic behavior Soils: Pore fluid response: Transient consolidation: toggle off Include creep/swelling/viscoelastic behavior IntegrationExplicit 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 schemesNonlinear creep problems are often solved efficiently by forwarddifference 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.
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 quasistatic and coupled temperaturedisplacement 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 temperaturedisplacement or quasistatic 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: VISCO, CREEP=EXPLICIT COUPLED TEMPERATUREDISPLACEMENT, CREEP=EXPLICIT Abaqus/CAE Usage Use one of the following options to restrict Abaqus/Standard to using explicit integration: Step module: Create Step: Visco: Incrementation: Creep/swelling/viscoelastic integration: Explicit Coupled tempdisplacement: toggle on Include creep/swelling/ viscoelastic behavior: Incrementation: Creep/swelling/viscoelastic integration: Explicit Automatic monitoring of stability limit during explicit integrationAbaqus/Standard monitors the stability limit automatically during explicit integration. If, at any point in the model, the creep strain increment $\left({{\dot{\overline{\epsilon}}}^{cr}}_{t}\mathrm{\Delta}t\right)$ is larger than the total elastic strain, the problem will become unstable. Therefore, a stable time step, $\mathrm{\Delta}{t}_{s}$, is calculated every increment by $$\mathrm{\Delta}{t}_{s}=0.5\frac{{{\epsilon}^{el}}_{t}}{{{\dot{\overline{\epsilon}}}^{cr}}_{t}},$$
where ${{\epsilon}^{el}}_{t}$ is the equivalent total elastic strain at time t, the beginning of the increment, and ${{\dot{\overline{\epsilon}}}^{cr}}_{t}$ is the equivalent creep strain rate at time t. Furthermore, $${{\epsilon}^{el}}_{t}=\frac{{\stackrel{~}{q}}_{t}}{\stackrel{~}{E}},$$
where ${\stackrel{~}{q}}_{t}$ is the Mises stress at time t, and $$\stackrel{~}{E}=2(1+\nu )(\mathbf{n}:{\mathbf{D}}^{el}:\mathbf{n})\approx 2.5\overline{E},$$
where
At every increment for which explicit integration is performed, the stable time increment, $\mathrm{\Delta}{t}_{s}$, is compared to the critical time increment, $\mathrm{\Delta}{t}_{c}$, which is calculated as follows: $$\mathrm{\Delta}{t}_{c}=\frac{errtol}{{{\dot{\overline{\epsilon}}}^{cr}}_{t+\mathrm{\Delta}t}{{\dot{\overline{\epsilon}}}^{cr}}_{t}}.$$
The quantity errtol is an error tolerance that you define as discussed below. If $\mathrm{\Delta}{t}_{s}$ is less than $\mathrm{\Delta}{t}_{c}$, $\mathrm{\Delta}{t}_{s}$ 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 $\mathrm{\Delta}{t}_{s}$ is less than $\mathrm{\Delta}{t}_{c}$ 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 $\ge 50\mathrm{\Delta}t$). The stiffness matrix will be reformed at every iteration if the implicit algorithm is used. Specifying the tolerance for automatic incrementationThe integration tolerance must be chosen so that increments in stress, $\mathrm{\u25b3}\mathit{\sigma}$, are calculated accurately. Consider a onedimensional example. The stress increment, $\mathrm{\u25b3}\sigma $, is $$\mathrm{\u25b3}\sigma =E\mathrm{\u25b3}{\epsilon}^{el}=E\left(\mathrm{\u25b3}\epsilon \mathrm{\u25b3}{\epsilon}^{cr}\right),$$
where $\mathrm{\u25b3}{\epsilon}^{el}$, $\mathrm{\u25b3}\epsilon $, and $\mathrm{\u25b3}{\epsilon}^{cr}$ are the uniaxial elastic, total, and creep strain increments, respectively, and E is the elastic modulus. For $\mathrm{\u25b3}\sigma $ to be calculated accurately, the error in the creep strain increment, $\mathrm{\u25b3}{\epsilon}_{err}^{cr}$, must be small compared to $\mathrm{\u25b3}{\epsilon}^{el}$; that is, $$\mathrm{\u25b3}{\epsilon}_{err}^{cr}\ll \mathrm{\u25b3}{\epsilon}^{el}.$$
Measuring the error in $\mathrm{\u25b3}{\epsilon}^{cr}$ as $$\mathrm{\u25b3}{\epsilon}_{err}^{cr}=\left({{\dot{\overline{\epsilon}}}^{cr}}_{t+\mathrm{\u25b3}t}{{\dot{\overline{\epsilon}}}^{cr}}_{t}\right)\mathrm{\u25b3}t$$
leads to $$\left({{\dot{\overline{\epsilon}}}^{cr}}_{t+\mathrm{\u25b3}t}{{\dot{\overline{\epsilon}}}^{cr}}_{t}\right)\mathrm{\u25b3}t\ll \mathrm{\u25b3}{\epsilon}^{el}=\frac{\mathrm{\u25b3}\sigma}{E},\u2006\mathrm{or}$$
$$errtol\ll \frac{\mathrm{\u25b3}\sigma}{E}.$$
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. Input File Usage Use one of the following options: VISCO, CETOL=errtol COUPLED TEMPERATUREDISPLACEMENT, CETOL=errtol SOILS, CONSOLIDATION, CETOL=errtol Abaqus/CAE Usage Use one of the following options: Step module: Create Step: Visco: Incrementation: toggle on Creep/swelling/viscoelastic strain error tolerance, and enter a value Coupled tempdisplacement: 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 rateIn 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 ${r}_{\mathrm{max}}$, 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 ${r}_{\mathrm{max}}$ 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: $$\begin{array}{cc}\hfill {r}_{\mathrm{max}}<0.2& p=2.0{p}_{\mathrm{old}},\text{or}\hfill \\ \hfill {r}_{\mathrm{max}}3.0& p=0.5{p}_{\mathrm{old}},\hfill \end{array}$$
where p is the new load magnitude and ${p}_{\mathrm{old}}$ is the old load magnitude. If $0.2\le {r}_{\mathrm{max}}\le 3.0$, the increment is accepted; and at the beginning of the following time increment, the load magnitudes are modified as follows: $$\begin{array}{cc}\hfill 0.2\le {r}_{\mathrm{max}}<0.5& \phantom{\rule{.8em}{0ex}}p=1.5{p}_{\mathrm{old}};\hfill \\ \hfill 0.5\le {r}_{\mathrm{max}}<0.8& \phantom{\rule{.8em}{0ex}}p=1.2{p}_{\mathrm{old}};\hfill \\ \hfill 0.8\le {r}_{\mathrm{max}}<1.5& \phantom{\rule{.8em}{0ex}}p={p}_{\mathrm{old}};\text{or}\hfill \\ \hfill 1.5\le {r}_{\mathrm{max}}\le 3.0& \phantom{\rule{.8em}{0ex}}p={p}_{\mathrm{old}}/\mathrm{1.2.}\hfill \end{array}$$
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. A solutiondependent amplitude is used to define the minimum and maximum limits of the loading (see Defining a solutiondependent amplitude for superplastic forming analysis). Any number or combination of loads can be used. The current value of ${r}_{\mathrm{max}}$ is available for output as discussed below. Input File Usage Use all of the following options: AMPLITUDE, NAME=name, DEFINITION=SOLUTION DEPENDENT CLOAD, DLOAD, DSLOAD, and/or BOUNDARY with AMPLITUDE=name CREEP STRAIN RATE CONTROL, AMPLITUDE=name, ELSET=elset 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. ElementsRatedependent 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. OutputIn 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:
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:
