김경종
308 lines
22 KiB
Markdown
308 lines
22 KiB
Markdown
<!-- source-page: 261 -->
|
||
|
||
steady-state condition is reached; that is, until the stress-strain curve no longer changes shape from one cycle to the next. Such a stabilized cycle is shown in Figure 23.2.2–9. Each data pair $( \sigma _ { i } , \varepsilon _ { i } ^ { p l } )$ must be specified with the strain axis shifted to $\varepsilon _ { p } ^ { 0 } ,$ , so that
|
||
|
||
$$
|
||
\varepsilon_ {i} ^ {p l} = \varepsilon_ {i} - \frac {\sigma_ {i}}{E} - \varepsilon_ {p} ^ {0},
|
||
$$
|
||
|
||
and, thus, $\varepsilon _ { 1 } ^ { p l } = 0$ .
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
σ
|
||
σ₁ σ₂ σᵢ σₙ
|
||
Δε
|
||
εᵢ
|
||
ε
|
||
εₚ⁰
|
||
εₚⁱ = εᵢ - σᵢ / E - εₚ⁰
|
||
</details>
|
||
|
||
Figure 23.2.2–9 Stress-strain data for a stabilized cycle.
|
||
|
||
For each pair $( \sigma _ { i } , \varepsilon _ { i } ^ { p l } )$ values of $\alpha _ { i } \ \left( \alpha _ { i } \right.$ is the overall backstress obtained by summing all the backstresses at this data point) are obtained from the test data as
|
||
|
||
$$
|
||
\alpha_ {i} = \sigma_ {i} - \sigma^ {s},
|
||
$$
|
||
|
||
where $\sigma ^ { s } = ( \sigma _ { 1 } + \sigma _ { n } ) / 2$ is the stabilized size of the yield surface.
|
||
|
||
Integration of the backstress evolution laws over this uniaxial strain cycle, with an exact match for the first data pair $( \sigma _ { 1 } , 0 )$ , provides the expressions
|
||
|
||
$$
|
||
\alpha_ {k} = \frac {C _ {k}}{\gamma_ {k}} (1 - e ^ {- \gamma_ {k} \varepsilon^ {p l}}) + \alpha_ {k, 1} e ^ {- \gamma_ {k} \varepsilon^ {p l}},
|
||
$$
|
||
|
||
where $\alpha _ { k , 1 }$ denotes the $k ^ { t h }$ backstress at the first data point (initial value of the $k ^ { t h }$ backstress). The above equations enable calibration of the parameters $C _ { k }$ and $\gamma _ { k }$ .
|
||
|
||
If the shapes of the stress-strain curves are significantly different for different strain ranges, you may want to obtain several calibrated values of $C _ { k }$ and $\gamma _ { k }$ . The tabular data of the stress-strain curves obtained at different strain ranges can be entered directly in Abaqus. Calibrated values corresponding to each strain range are reported in the data file, together with an averaged set of parameters, if model definition data are requested (see “Controlling the amount of analysis input file processor information written to the
|
||
|
||
<!-- source-page: 262 -->
|
||
|
||
data file” in “Output,” Section 4.1.1). Abaqus will use the averaged set in the analysis. These parameters may have to be adjusted to improve the match to the test data at the strain range anticipated in the analysis.
|
||
|
||
When test data are given as functions of temperature and/or field variables, Abaqus determines several sets of material parameters $( C _ { 1 } , \gamma _ { 1 } , . . . , C _ { N } , \gamma _ { N } )$ , each corresponding to a given combination of temperature and/or field variables. Generally, this results in temperature-history (and/or field variablehistory) dependent material behavior because the values of vary with changes in temperature and/or field variables. This dependency on temperature-history is small and fades away with increasing plastic deformation. However, you can make the response of the material completely independent of the history of temperature and field variables by using constant values for the parameters $\gamma _ { k }$ . This can be achieved by running a data check analysis first; an appropriate constant values of $\gamma _ { k }$ can be determined from the information provided in the data file during the data check. The values for the parameters $C _ { k }$ and the constant parameters $\gamma _ { k }$ can then be entered directly as described above.
|
||
|
||
If the model with multiple backstresses is used, Abaqus obtains hardening parameters for different values of initial guesses and chooses the ones that give the best correlation with the experimental data provided. However, you should carefully examine the obtained parameters. In some cases it might be advantageous to obtain hardening parameters for different numbers of backstresses before choosing the set of parameters.
|
||
|
||
The isotropic hardening component should be defined by specifying the equivalent stress defining the size of the yield surface at zero plastic strain, as well as the evolution of the equivalent stress as a function of equivalent plastic strain. If this component is not defined, Abaqus will assume that no cyclic hardening occurs so that the equivalent stress defining the size of the yield surface is constant and equal to $( \sigma _ { 1 } + \sigma _ { n } ) / 2$ (or the average of these quantities over several strain ranges when more than one strain range is provided). Since this size corresponds to the size of a saturated cycle, this is unlikely to provide accurate predictions of actual behavior, particularly in the initial cycles.
|
||
|
||
Input File Usage: \*PLASTIC, HARDENING=COMBINED, DATA TYPE=STABILIZED, NUMBER BACKSTRESSES=n
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Combined, Data type: Stabilized, Number of backstresses: n
|
||
|
||
# Initial conditions
|
||
|
||
When we need to study the behavior of a material that has already been subjected to some hardening, Abaqus allows you to prescribe initial conditions for the equivalent plastic strain, $\bar { \varepsilon } ^ { p l }$ , and for the backstresses, $\alpha _ { k }$ . When the nonlinear isotropic/kinematic hardening model is used, the initial conditions for each backstress, $\alpha _ { k }$ , must satisfy the condition
|
||
|
||
$$
|
||
\sqrt {\frac {3}{2} \alpha_ {k} ^ {d e v} : \alpha_ {k} ^ {d e v}} \leq C _ {k} / \gamma_ {k}
|
||
$$
|
||
|
||
for the model to produce a kinematic hardening response. Abaqus allows the specification of initial backstresses that violate these conditions. However, in this case the response corresponding to the backstress for which the condition is violated produces kinematic softening response: the magnitude
|
||
|
||
<!-- source-page: 263 -->
|
||
|
||
of the backstress decreases with plastic straining from its initial value to the saturation value. If the condition is violated for any of the backstresses, the overall response of the material is not guaranteed to produce kinematic hardening response. The initial condition for the backstress has no limitations when the linear kinematic hardening model is used.
|
||
|
||
You can specify the initial values of $\bar { \varepsilon } ^ { p l }$ and $\alpha _ { k }$ directly as initial conditions (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING, NUMBER BACKSTRESSES=n
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Number of backstresses: n
|
||
|
||
# User subroutine specification in Abaqus/Standard
|
||
|
||
For more complicated cases in Abaqus/Standard initial conditions can be defined through user subroutine HARDINI.
|
||
|
||
Input File Usage: \*INITIAL CONDITIONS, TYPE=HARDENING, USER, NUMBER BACKSTRESSES=n
|
||
|
||
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined, Number of backstresses: n
|
||
|
||
# Elements
|
||
|
||
These models can be used with elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom), except some beam elements in space. Beam elements in space that include shear stress caused by torsion (i.e., not thin-walled, open sections) and do not include hoop stress (i.e., not PIPE elements) cannot be used with the nonlinear kinematic hardening model. In Abaqus/Explicit the kinematic hardening models can be used with any elements that include mechanical behavior, with the exception of one-dimensional elements (beams, pipes, and trusses) when the models are used with the Hill yield surface.
|
||
|
||
# Output
|
||
|
||
In addition to the standard output identifiers available in Abaqus (“Abaqus/Standard output variable identifiers,” Section 4.2.1, and “Abaqus/Explicit output variable identifiers,” Section 4.2.2), the following variables have special meaning for the kinematic hardening models:
|
||
|
||
ALPHA Total kinematic hardening shift tensor components, $\alpha _ { i j } ( i , j \leq 3 )$ .
|
||
|
||
ALPHAk $k ^ { t h }$ kinematic hardening shift tensor components $( 1 \leq k \leq 1 0 )$ .
|
||
|
||
ALPHAN All tensor components of all the kinematic hardening shift tensors, except the total shift tensor.
|
||
|
||
<!-- source-page: 264 -->
|
||
|
||
PEEQ Equivalent plastic strain, $\begin{array} { r l r } { \bar { \varepsilon } ^ { p l } } & { { } = } & { \bar { \varepsilon } ^ { p l } | _ { 0 } + \int _ { 0 } ^ { t } \frac { \pmb { \sigma } : \dot { \varepsilon } ^ { p l } d t } { \sigma ^ { 0 } } } \end{array}$ 90 where $\bar { \varepsilon } ^ { p l } | _ { 0 }$ is the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”).
|
||
|
||
PENER Plastic work, defined as: $\begin{array} { r } { W ^ { p l } \ = \ \int _ { 0 } ^ { t } { \pmb \sigma } : \dot { \varepsilon } ^ { p l } d t . } \end{array}$ . This quantity is not guaranteed to be monotonically increasing for kinematic hardening models. To get a quantity that is monotonically increasing, the plastic dissipation needs to be computed as: $\begin{array} { r } { W ^ { p l } \ = \ \int _ { 0 } ^ { t } \left( \pmb { \sigma } - \pmb { \alpha } \right) : \dot { \varepsilon } ^ { p l } d t } \end{array}$ . In Abaqus/Standard this quantity can be computed as a user-defined output variable in user subroutine UVARM.
|
||
|
||
YIELDS Yield stress, $\sigma ^ { 0 }$ .
|
||
|
||
<!-- source-page: 265 -->
|
||
|
||
# 23.2.3 RATE-DEPENDENT YIELD
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Classical metal plasticity,” Section 23.2.1
|
||
• “Models for metals subjected to cyclic loading,” Section 23.2.2
|
||
• “Johnson-Cook plasticity,” Section 23.2.7
|
||
• “Extended Drucker-Prager models,” Section 23.3.1
|
||
• “Crushable foam plasticity models,” Section 23.3.5
|
||
• “Material library: overview,” Section 21.1.1
|
||
• “Inelastic behavior,” Section 23.1.1
|
||
• \*RATE DEPENDENT
|
||
• “Defining rate-dependent yield with yield stress ratios” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
Rate-dependent yield:
|
||
|
||
• is needed to define a material’s yield behavior accurately when the yield strength depends on the rate of straining and the anticipated strain rates are significant;
|
||
• is available only for the isotropic hardening metal plasticity models (Mises and Johnson-Cook), the isotropic component of the nonlinear isotropic/kinematic plasticity models, the extended Drucker-Prager plasticity model, and the crushable foam plasticity model;
|
||
• can be conveniently defined on the basis of work hardening parameters and field variables by providing tabular data for the isotropic hardening metal plasticity models, the isotropic component of the nonlinear isotropic/kinematic plasticity models, and the extended Drucker-Prager plasticity model;
|
||
• can be defined through specification of user-defined overstress power law parameters, yield stress ratios, or Johnson-Cook rate dependence parameters (this last option is not available for the crushable foam plasticity model and is the only option available for the Johnson-Cook plasticity model);
|
||
• cannot be used with any of the Abaqus/Standard creep models (metal creep, time-dependent volumetric swelling, Drucker-Prager creep, or cap creep) since creep behavior is already a rate-dependent mechanism; and
|
||
• in dynamic analysis should be specified such that the yield stress increases with increasing strain rate.
|
||
|
||
<!-- source-page: 266 -->
|
||
|
||
# Work hardening dependencies
|
||
|
||
Generally, a material’s yield stress, (or for the crushable foam model), is dependent on work hardening, which for isotropic hardening models is usually represented by a suitable measure of equivalent plastic strain, $\bar { \varepsilon } ^ { p l }$ ; the inelastic strain rate, $\dot { \bar { \varepsilon } } ^ { p l }$ ; temperature, $\theta ;$ and predefined field variables, $f _ { i } { \mathrm { : } }$
|
||
|
||
$$
|
||
\bar {\sigma} = \bar {\sigma} (\bar {\varepsilon} ^ {p l}, \dot {\bar {\varepsilon}} ^ {p l}, \theta , f _ {i}).
|
||
$$
|
||
|
||
Many materials show an increase in their yield strength as strain rates increase; this effect becomes important in many metals and polymers when the strain rates range between 0.1 and 1 per second, and it can be very important for strain rates ranging between 10 and 100 per second, which are characteristic of high-energy dynamic events or manufacturing processes.
|
||
|
||
# Defining hardening dependencies for various material models
|
||
|
||
Strain rate dependence can be defined by entering hardening curves at different strain rates directly or by defining yield stress ratios to specify the rate dependence independently.
|
||
|
||
# Direct entry of test data
|
||
|
||
Work hardening dependencies can be given quite generally as tabular data for the isotropic hardening Mises plasticity model, the isotropic component of the nonlinear isotropic/kinematic hardening model, and the extended Drucker-Prager plasticity model. The test data are entered as tables of yield stress values versus equivalent plastic strain at different equivalent plastic strain rates. The yield stress must be given as a function of the equivalent plastic strain and, if required, of temperature and of other predefined field variables. In defining this dependence at finite strains, “true” (Cauchy) stress and log strain values should be used. The hardening curve at each temperature must always start at zero plastic strain. For perfect plasticity only one yield stress, with zero plastic strain, should be defined at each temperature. It is possible to define the material to be strain softening as well as strain hardening. The work hardening data are repeated as often as needed to define stress-strain curves at different strain rates. The yield stress at a given strain and strain rate is interpolated directly from these tables.
|
||
|
||
Input File Usage: Use one of the following options:
|
||
|
||
\*PLASTIC, HARDENING=ISOTROPIC, RATE=
|
||
\*CYCLIC HARDENING, RATE=
|
||
\*DRUCKER PRAGER HARDENING, RATE=
|
||
|
||
Abaqus/CAE Usage: Use one of the following models:
|
||
|
||
Property module: material editor:
|
||
|
||
Mechanical→Plasticity→Plastic: Hardening: Isotropic,
|
||
|
||
Use strain-rate-dependent data
|
||
|
||
Mechanical→Plasticity→Drucker Prager: Suboptions→Drucker
|
||
|
||
Prager Hardening: Use strain-rate-dependent data
|
||
|
||
Cyclic hardening is not supported in Abaqus/CAE.
|
||
|
||
<!-- source-page: 267 -->
|
||
|
||
# Using yield stress ratios
|
||
|
||
Alternatively, and as the only means of defining rate-dependent yield stress for the Johnson-Cook and the crushable foam plasticity models, the strain rate behavior can be assumed to be separable, so that the stress-strain dependence is similar at all strain rate levels:
|
||
|
||
$$
|
||
\bar {\sigma} = \sigma^ {0} (\bar {\varepsilon} ^ {p l}, \theta , f _ {i}) R (\dot {\bar {\varepsilon}} ^ {p l}, \theta , f _ {i}),
|
||
$$
|
||
|
||
where $\sigma ^ { 0 } ( \bar { \varepsilon } ^ { p l } , \theta , f _ { i } )$ (or $B ( \bar { \varepsilon } ^ { p l } , \theta , f _ { i } )$ in the foam model) is the static stress-strain behavior and $R ( \dot { \bar { \varepsilon } } ^ { p l } , \theta , f _ { i } )$ is the ratio of the yield stress at nonzero strain rate to the static yield stress (so that $R ( 0 , \theta , f _ { i } ) = 1 . 0 )$ .
|
||
|
||
Three methods are offered to define R in Abaqus: specifying an overstress power law, defining R directly as a tabular function, or specifying an analytical Johnson-Cook form to define R.
|
||
|
||
# Overstress power law
|
||
|
||
The Cowper-Symonds overstress power law has the form
|
||
|
||
$$
|
||
\dot {\bar {\varepsilon}} ^ {p l} = D (R - 1) ^ {n} \quad \text {for} \quad \bar {\sigma} \geq \sigma^ {0} \quad \text {(or} \quad \bar {B} \geq B \quad \text {in the crushable foam model),}
|
||
$$
|
||
|
||
where $D ( \theta , f _ { i } )$ and $n ( \theta , f _ { i } )$ are material parameters that can be functions of temperature and, possibly, of other predefined field variables.
|
||
|
||
Input File Usage: \*RATE DEPENDENT, TYPE=POWER LAW
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Suboptions→Rate Dependent:
|
||
|
||
Hardening: Power Law (available for valid plasticity models)
|
||
|
||
# Tabular function
|
||
|
||
Alternatively, R can be entered directly as a tabular function of the equivalent plastic strain rate (or the axial plastic strain rate in a uniaxial compression test for the crushable foam model), $\dot { \bar { \varepsilon } } ^ { p l }$ ; temperature, $\theta ;$ and field variables, $f _ { i }$ .
|
||
|
||
Input File Usage: \*RATE DEPENDENT, TYPE=YIELD RATIO
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Suboptions→Rate Dependent:
|
||
|
||
Hardening: Yield Ratio (available for valid plasticity models)
|
||
|
||
# Johnson-Cook rate dependence
|
||
|
||
Johnson-Cook rate dependence has the form
|
||
|
||
$$
|
||
\dot {\bar {\varepsilon}} ^ {p l} = \dot {\varepsilon} _ {0} \mathrm{exp} \left[ \frac {1}{C} (R - 1) \right] \quad \mathrm{for} \quad \bar {\sigma} \geq \sigma^ {0},
|
||
$$
|
||
|
||
where $\dot { \varepsilon } _ { 0 }$ and $c$ are material constants that do not depend on temperature and are assumed not to depend on predefined field variables. Johnson-Cook rate dependence can be used in conjunction with the Johnson-Cook plasticity model, the isotropic hardening metal plasticity models, and the extended
|
||
|
||
<!-- source-page: 268 -->
|
||
|
||
Drucker-Prager plasticity model (it cannot be used in conjunction with the crushable foam plasticity model).
|
||
|
||
This is the only form of rate dependence available for the Johnson-Cook plasticity model. For more details, see “Johnson-Cook plasticity,” Section 23.2.7.
|
||
|
||
Input File Usage: \*RATE DEPENDENT, TYPE=JOHNSON COOK
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Suboptions→Rate Dependent:
|
||
|
||
Hardening: Johnson-Cook (available for valid plasticity models)
|
||
|
||
# Elements
|
||
|
||
Rate-dependent yield can be used with all elements that include mechanical behavior (elements that have displacement degrees of freedom).
|
||
|
||
<!-- source-page: 269 -->
|
||
|
||
# 23.2.4 RATE-DEPENDENT PLASTICITY: CREEP AND SWELLING
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Material library: overview,” Section 21.1.1
|
||
• “Inelastic behavior,” Section 23.1.1
|
||
• “Defining the gasket behavior directly using a gasket behavior model,” Section 32.6.6
|
||
• \*CREEP
|
||
• \*CREEP STRAIN RATE CONTROL
|
||
• \*POTENTIAL
|
||
• \*SWELLING
|
||
• \*RATIOS
|
||
• “Defining a creep law” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining swelling” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
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,” Section 23.2.12);
|
||
• 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).
|
||
|
||
<!-- source-page: 270 -->
|
||
|
||
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 thicknessdirection 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
|
||
|
||
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,” Section 21.1.2). 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:
|
||
|
||
\*MATERIAL \*CREEP
|
||
|
||
Use the following options to define creep in conjunction with gasket behavior:
|
||
|
||
\*GASKET BEHAVIOR \*CREEP
|
||
|
||
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Creep
|
||
|
||
# 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 and/or field dependencies, the time-hardening and
|