김경종
292 lines
21 KiB
Markdown
292 lines
21 KiB
Markdown
<!-- source-page: 321 -->
|
||
|
||
# 23.2.11 TWO-LAYER VISCOPLASTICITY
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Material library: overview,” Section 21.1.1
|
||
• “Combining material behaviors,” Section 21.1.3
|
||
• “Inelastic behavior,” Section 23.1.1
|
||
• \*ELASTIC
|
||
• \*PLASTIC
|
||
• \*VISCOUS
|
||
• “Defining the viscous component of a two-layer viscoplasticity model” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
The two-layer viscoplastic model:
|
||
|
||
• is intended for modeling materials in which significant time-dependent behavior as well as plasticity is observed, which for metals typically occurs at elevated temperatures;
|
||
• consists of an elastic-plastic network that is in parallel with an elastic-viscous network (in contrast to the coupled creep and plasticity capabilities in which the plastic and the viscous networks are in series);
|
||
• is based on a Mises or Hill yield condition in the elastic-plastic network and any of the available creep models in Abaqus/Standard (except the hyperbolic creep law) in the elastic-viscous network;
|
||
• assumes a deviatoric inelastic response (hence, the pressure-dependent plasticity or creep models cannot be used to define the behavior of the two networks);
|
||
• is intended for modeling material response under fluctuating loads over a wide range of temperatures; and
|
||
• has been shown to provide good results for thermomechanical loading.
|
||
|
||
# Material behavior
|
||
|
||
The material behavior is broken down into three parts: elastic, plastic, and viscous. Figure 23.2.11–1 shows a one-dimensional idealization of this material model, with the elastic-plastic and the elasticviscous networks in parallel. The following subsections describe the elastic and the inelastic (plastic and viscous) behavior in detail.
|
||
|
||
<!-- source-page: 322 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>chemical</summary>
|
||
|
||
Electrical circuit diagram with resistors, inductors, and a capacitor labeled with symbols Kp, H', σγ, Kv, and η, m
|
||
</details>
|
||
|
||
Figure 23.2.11–1 One-dimensional idealization of the two-layer viscoplasticity model.
|
||
|
||
# Elastic behavior
|
||
|
||
The elastic part of the response for both networks is specified using a linear isotropic elasticity definition. Any one of the available elasticity models in Abaqus/Standard can be used to define the elastic behavior of the networks. Referring to the one-dimensional idealization (Figure 23.2.11–1), the ratio of the elastic modulus of the elastic-viscous network $( K _ { V } )$ to the total (instantaneous) modulus $( K _ { P } + K _ { V } )$ is given by
|
||
|
||
$$
|
||
f = \frac {K _ {V}}{(K _ {P} + K _ {V})}.
|
||
$$
|
||
|
||
The user-specified ratio $f ,$ given as part of the viscous behavior definition as discussed later, apportions the total moduli specified for the elastic behavior among the elastic-viscous and the elastic-plastic networks. As a result, if isotropic elastic properties are defined, the Poisson’s ratios are the same in both networks. On the other hand, if anisotropic elasticity is defined, the same type of anisotropy holds for both networks. The properties specified for the elastic behavior are assumed to be the instantaneous properties $( K _ { P } +$ $K _ { V } )$ .
|
||
|
||
Input File Usage: \*ELASTIC
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Elasticity→Elastic
|
||
|
||
# Plastic behavior
|
||
|
||
A plasticity definition can be used to provide the static hardening data for the material model. All available metal plasticity models, including Hill’s plasticity model to define anisotropic yield (“Anisotropic yield/creep,” Section 23.2.6), can be used.
|
||
|
||
The elastic-plastic network does not take into account rate-dependent yield. Hence, any specification of strain rate dependence for the plasticity model is not allowed.
|
||
|
||
<!-- source-page: 323 -->
|
||
|
||
Input File Usage: Use the following options:
|
||
|
||
\*PLASTIC
|
||
|
||
\*POTENTIAL
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Potential
|
||
|
||
# Viscous behavior
|
||
|
||
The viscous behavior of the material can be governed by any of the available creep laws in Abaqus/Standard (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), except the hyperbolic creep law. When you define the viscous behavior, you specify the viscosity parameters and choose the specific type of viscous behavior. If you choose to input the creep law through user subroutine CREEP, only deviatoric creep should be defined—more specifically, volumetric swelling behavior should not be defined within user subroutine CREEP. In addition, you also specify the fraction, f, that defines the ratio of the elastic modulus of the elastic-viscous network to the total (instantaneous) modulus. Viscous stress ratios can be specified under the viscous behavior definition to define anisotropic viscosity (see “Anisotropic yield/creep,” Section 23.2.6).
|
||
|
||
All material properties can be specified as functions of temperature and predefined field variables.
|
||
|
||
Input File Usage: Use the following options:
|
||
|
||
\*VISCOUS, LAW=TIME or STRAIN or USER or ANAND
|
||
|
||
or DARVEAUX or DOUBLE POWER
|
||
|
||
\*POTENTIAL
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Viscous: Suboptions→Potential: Time, Strain, or User
|
||
|
||
Specifying the Anand, Darveaux, and double power creep laws is not supported in Abaqus/CAE.
|
||
|
||
# Time-dependent behavior
|
||
|
||
In 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 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.
|
||
|
||
Input File Usage: Use one of the following options:
|
||
|
||
\*VISCOUS, TIME=TOTAL (default)
|
||
|
||
\*VISCOUS, TIME=CREEP
|
||
|
||
Abaqus/CAE Usage: Specifying the time type is not supported in Abaqus/CAE.
|
||
|
||
<!-- source-page: 324 -->
|
||
|
||
# Thermal expansion
|
||
|
||
Thermal expansion can be modeled by providing the thermal expansion coefficient of the material (“Thermal expansion,” Section 26.1.2). Anisotropic expansion can be defined in the usual manner. In the one-dimensional idealization the expansion element is assumed to be in series with the rest of the network.
|
||
|
||
# Calibration of material parameters
|
||
|
||
The calibration procedure is best explained in the context of the one-dimensional idealization of the material model. In the following discussion the viscous behavior is assumed to be governed by the Norton-Hoff rate law, which is given by
|
||
|
||
$$
|
||
\dot {\varepsilon} _ {V} ^ {v} = A \sigma_ {V} ^ {n}.
|
||
$$
|
||
|
||
In the expression above the subscript V denotes quantities in the elastic-viscous network alone. This form of the rate law may be chosen, for example, by choosing a time-hardening power law for the viscous behavior and setting $m = 0$ . For this basic case there are six material parameters that need to be calibrated (Figure 23.2.11–1). These are the elastic properties of the two networks, $K _ { P }$ and $K _ { V } ;$ the initial yield stress $\sigma _ { y }$ ; the hardening $H ^ { ' }$ ; and the Norton-Hoff rate parameters, A and n.
|
||
|
||
The experiment that needs to be performed is uniaxial tension under different constant strain rates. A static (effectively zero strain rate) uniaxial tension test determines the long-term modulus, $K _ { P } ;$ the initial yield stress, $\sigma _ { y }$ ; and the hardening, $H ^ { ' }$ . The hardening is assumed to be linear for illustration purposes. The material model is not limited to linear hardening, and any general hardening behavior can be defined for the plasticity model. The instantaneous elastic modulus, $K = K _ { P } + K _ { V }$ , can be measured by measuring the initial elastic response of the material under nonzero, relatively high, strain rates. Several such measurements at different applied strain rates can be compared until the instantaneous moduli does not change with a change in the applied strain rate. The difference between K and $K _ { P }$ determines $K _ { V }$ .
|
||
|
||
To calibrate the parameters A and n, it is useful to recognize that the long-term (steady-state) behavior of the elastic-viscous network under a constant applied strain rate, $\dot { \varepsilon } _ { o } ,$ , is a constant stress of magnitude $\sigma _ { V } = A ^ { - \frac { 1 } { n } } \dot { \varepsilon } _ { o } ^ { \frac { 1 } { n } }$ . Under the assumption that the hardening modulus is negligible compared to the elastic modulus $( K _ { P } > > H ^ { ' } )$ , the steady-state response of the overall material is given by
|
||
|
||
$$
|
||
\sigma = A ^ {- \frac {1}{n}} \dot {\varepsilon} _ {o} ^ {\frac {1}{n}} + \sigma_ {y} + H ^ {'} \varepsilon ,
|
||
$$
|
||
|
||
where $\sigma$ is the total stress for a given total strain . To determine whether steady state has been reached, one can plot the quantity $\boldsymbol { \bar { \sigma } } = \boldsymbol { \sigma } - \boldsymbol { \sigma _ { y } } - \boldsymbol { H } ^ { \prime }$ as a function of and note when it becomes a constant. The constant value of is equal to $A ^ { - \frac { 1 } { n } } \dot { \varepsilon } _ { o } ^ { \frac { 1 } { n } }$ . By performing several tests at different values of the constant applied strain rate $\dot { \varepsilon } _ { o }$ , it is possible to determine the constants A and n.
|
||
|
||
<!-- source-page: 325 -->
|
||
|
||
The material is active during all stress/displacement procedure types. In a static analysis step where the long-term response is requested (see “Static stress analysis,” Section 6.2.2), only the elastic-plastic network will be active; the elastic-viscous network will not contribute in any manner. In particular, the stress in the viscous network will be zero during a long-term static response. If the creep effects are removed in a coupled temperature-displacement procedure or a soils consolidation procedure, the response of the elastic-viscous network will be assumed to be elastic only. During a linear perturbation step, only the elastic response of the networks is considered.
|
||
|
||
Some stress/displacement procedure types (coupled temperature-displacement, soils consolidation, and quasi-static) allow user control of the time integration accuracy of the viscous constitutive equations through a user-specified error tolerance. In other procedure types where no such direct control is currently available (static, dynamic), you must choose appropriate time increments. These time increments must be small compared to the typical relaxation time of the material.
|
||
|
||
# Elements
|
||
|
||
The two-layer viscoplastic model is not available for one-dimensional elements (beams and trusses). It can be used with any other element in Abaqus/Standard that includes mechanical behavior (elements that have displacement degrees of freedom).
|
||
|
||
# Output
|
||
|
||
In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), the following variables have special meaning for the two-layer viscoplastic material model:
|
||
|
||
EE The elastic strain is defined as: $\varepsilon ^ { e l } = f \varepsilon _ { V } ^ { e l } + ( 1 - f ) \varepsilon _ { P } ^ { e l }$
|
||
|
||
PE Plastic strain, $\varepsilon _ { P } ^ { p l }$ , in the elastic-plastic network.
|
||
|
||
VE Viscous strain, $\varepsilon _ { V } ^ { v }$ , in the elastic-viscous network.
|
||
|
||
PS Stress, $\sigma _ { P }$ , in the elastic-plastic network.
|
||
|
||
VS Stress, $\pmb { \sigma } _ { V }$ , in the elastic-viscous network.
|
||
|
||
PEEQ The equivalent plastic strain, defined as $\begin{array} { r } { \int _ { 0 } ^ { t } \sqrt { \frac { 2 } { 3 } \dot { \varepsilon } _ { P } ^ { p l } : \dot { \varepsilon } _ { P } ^ { p l } } d t } \end{array}$
|
||
|
||
VEEQ The equivalent viscous strain, defined as $\begin{array} { r } { \int _ { 0 } ^ { t } \sqrt { \frac { 2 } { 3 } \dot { \varepsilon } _ { V } ^ { v } : \dot { \varepsilon } _ { V } ^ { v } } d t . } \end{array}$
|
||
|
||
SENER The elastic strain energy density per unit volume, defined as ${ \textstyle \frac { 1 } { 2 } } { \pmb \sigma } _ { P } : \varepsilon _ { P } ^ { e l } + { \textstyle \frac { 1 } { 2 } } { \pmb \sigma } _ { V } : \varepsilon _ { V } ^ { e l }$ .
|
||
|
||
PENER The plastic dissipated energy per unit volume, defined as $\int _ { 0 } ^ { t } { \pmb { \sigma } } _ { P } : \dot { \varepsilon } _ { P } ^ { p l } d t$ .
|
||
|
||
VENER The viscous dissipated energy per unit volume, defined as $\textstyle \int _ { 0 } ^ { t } { \pmb { \sigma } } _ { V } : { \dot { \varepsilon } } _ { V } ^ { v } d t$
|
||
|
||
The above definitions of the strain tensors imply that the total strain is related to the elastic, plastic, and viscous strains through the following relation:
|
||
|
||
<!-- source-page: 326 -->
|
||
|
||
$$
|
||
\varepsilon = \varepsilon^ {e l} + (1 - f) \varepsilon^ {p l} + f \varepsilon^ {v},
|
||
$$
|
||
|
||
where according to the definitions given above $\varepsilon ^ { p l } = \varepsilon _ { P } ^ { p l }$ and $\varepsilon ^ { v } = \varepsilon _ { V } ^ { v }$ . The above definitions of the output variables apply to all procedure types. In particular, when the long-term response is requested for a static procedure, the elastic-viscous network does not carry any stress and the definition of the elastic strain reduces to $\varepsilon ^ { e l } = ( 1 - f ) \varepsilon _ { P } ^ { e l }$ , which implies that the total stress is related to the elastic strain through the instantaneous elastic moduli.
|
||
|
||
# Additional reference
|
||
|
||
• Kichenin, J., “Comportement Thermomécanique du Polyéthylène—Application aux Structures Gazières,” Thèse de Doctorat de l’Ecole Polytechnique, Spécialité: Mécanique et Matériaux, 1992.
|
||
|
||
<!-- source-page: 327 -->
|
||
|
||
# 23.2.12 ORNL – OAK RIDGE NATIONAL LABORATORY CONSTITUTIVE MODEL
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Material library: overview,” Section 21.1.1
|
||
• “Inelastic behavior,” Section 23.1.1
|
||
• “Classical metal plasticity,” Section 23.2.1
|
||
• “Rate-dependent plasticity: creep and swelling,” Section 23.2.4
|
||
• \*ORNL
|
||
• \*PLASTIC
|
||
• \*CREEP
|
||
• “Using the Oak Ridge National Laboratory (ORNL) constitutive model in plasticity and creep calculations” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Specifying cycled yield stress data for the ORNL model” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
The Oak Ridge National Laboratory (ORNL) constitutive model:
|
||
|
||
• allows for use of the rules defined in the Nuclear Standard NEF 9–5T, “Guidelines and Procedures for Design of Class 1 Elevated Temperature Nuclear System Components,” in plasticity and creep calculations;
|
||
• is intended for use in modeling types 304 and 316 stainless steel at relatively high temperatures;
|
||
• can be used only with the metal plasticity models (linear kinematic hardening only) and/or the strain hardening form of the metal creep law; and
|
||
• is described in detail in “ORNL constitutive theory,” Section 4.3.8 of the Abaqus Theory Guide.
|
||
|
||
# Usage with plasticity
|
||
|
||
The ORNL constitutive model in Abaqus/Standard is based on the March 1981 issue of the Nuclear Standard NEF 9–5T and on the October 1986 issue, which revises the constitutive model extensively. This model adds isotropic hardening of the plastic yield surface from a virgin material state to a fully cycled state. Initially the material is assumed to harden kinematically according to a bilinear representation of the virgin stress-strain curve. If a strain reversal takes place or if the creep strain reaches 0.2%, the yield surface expands isotropically to the user-defined tenth-cycle stress-strain curve. Further hardening occurs kinematically according to a bilinear representation of the tenth-cycle stress-strain curve.
|
||
|
||
<!-- source-page: 328 -->
|
||
|
||
You must specify the virgin yield stress and the hardening through a plasticity model definition and the elastic part of the response through a linear elasticity model definition. You specify the tenth-cycle yield stress and hardening values separately. The yield stress at each temperature should be defined by giving its value at zero plastic strain and at one additional nonzero plastic strain point, thus giving a constant hardening rate (linear work hardening).
|
||
|
||
Input File Usage: Use all of the following options in the same material data block:
|
||
|
||
\*PLASTIC
|
||
|
||
\*ORNL
|
||
|
||
\*CYCLED PLASTIC
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Suboptions→Ornl and Suboptions→Cycled Plastic
|
||
|
||
Abaqus/Standard also allows you to invoke the optional kinematic shift ( ) reset procedure that is described in Section 4.3.5 of the Nuclear Standard. If you do not specify the reset procedure explicitly, it is not used.
|
||
|
||
Input File Usage: \*ORNL, RESET
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Suboptions→Ornl: Invoke reset procedure
|
||
|
||
# Usage with creep
|
||
|
||
The ORNL constitutive model assumes that creep uses the strain hardening formulation. It introduces auxiliary hardening rules when strain reversals occur. An algorithm providing details is presented in “ORNL constitutive theory,” Section 4.3.8 of the Abaqus Theory Guide. It can be used only when the creep behavior is defined by a strain-hardening power law.
|
||
|
||
Input File Usage: Use both of the following options in the same material data block:
|
||
|
||
\*CREEP, LAW=STRAIN
|
||
|
||
\*ORNL
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Creep:
|
||
|
||
Law: Strain-Hardening: Suboptions→Ornl
|
||
|
||
# Translation of the yield surface during creep
|
||
|
||
The ORNL formulation can also cause the center of the yield surface to translate during creep for use in subsequent plastic increments; this behavior is defined through two optional user-defined parameters.
|
||
|
||
# Specifying saturation rates for kinematic shift
|
||
|
||
You can specify A, the saturation rates for kinematic shift caused by creep strain as defined by Equation (15) of Section 4.3.3–3 of the Nuclear Standard. The default value is 0.3. Set A=0.0 to use the 1986 revision of the standard.
|
||
|
||
Input File Usage: \*ORNL, A=A
|
||
|
||
<!-- source-page: 329 -->
|
||
|
||
# Abaqus/CAE Usage: Property module: material editor: Suboptions→Ornl: Saturation rates for kinematic shift: A
|
||
|
||
# Specifying the rate of kinematic shift
|
||
|
||
You can specify H, the rate of kinematic shift with respect to creep strain (Equation (7) of Section 4.3.2–1 of the Nuclear Standard). Set H=0.0 to use the 1986 revision of the standard. If you do not specify a value for H, it is determined according to Section 4.3.3–3 of the 1981 revision of the standard.
|
||
|
||
Input File Usage: \*ORNL, H=H
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Suboptions→Ornl: Rate of kinematic shift wrt creep strain: H
|
||
|
||
# Initial conditions
|
||
|
||
When we need to study the behavior of a material that has already been subjected to some work hardening, initial equivalent plastic strain values can be provided to specify the yield stress corresponding to the work hardened state. See “Inelastic behavior,” Section 23.1.1, for additional details. Initial values can also be provided for the backstress tensor, , to include strain-induced anisotropy. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1, for more information. For more complicated cases initial conditions can be defined through user subroutine HARDINI.
|
||
|
||
Input File Usage: Use the following option to specify the initial equivalent plastic strain directly: \*INITIAL CONDITIONS, TYPE=HARDENING
|
||
|
||
Use the following option in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI:
|
||
|
||
\*INITIAL CONDITIONS, TYPE=HARDENING, USER
|
||
|
||
Abaqus/CAE Usage: Use the following options to specify the initial equivalent plastic strain directly:
|
||
|
||
Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step
|
||
|
||
Use the following options in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI:
|
||
|
||
Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined
|
||
|
||
# Elements
|
||
|
||
The ORNL constitutive model can be used with any elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom).
|
||
|
||
<!-- source-page: 330 -->
|
||
|
||
# Output
|
||
|
||
In addition to the standard output identifiers available in Abaqus/Standard (“Abaqus/Standard output variable identifiers,” Section 4.2.1), variables associated with creep (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4) and the kinematic hardening plasticity models (“Models for metals subjected to cyclic loading,” Section 23.2.2) are available for the ORNL constitutive model.
|