김경종
24 KiB
r _ {y} = \frac {d \varepsilon_ {1 1}}{d \varepsilon_ {3 3}} = \frac {H}{F}.
Transverse anisotropy
A transversely anisotropic material is one where r _ { x } = r _ { y } . If we define \sigma ^ { 0 } in the metal plasticity model to be equal to \bar { \sigma } _ { 1 1 } ,
R _ {1 1} = R _ {2 2} = 1
and, using the relationships above,
R _ {3 3} = \sqrt {\frac {r _ {x} + 1}{2}}.
If r _ { x } = 1 (isotropic material), R _ { 3 3 } = 1 and the Mises isotropic plasticity model is recovered.
Planar anisotropy
In the case of planar anisotropy r _ { x } and r _ { y } are different and R _ { 1 1 } , R _ { 2 2 } , R _ { 3 3 } will all be different. If we define \sigma ^ { 0 } in the metal plasticity model to be equal to \bar { \sigma } _ { 1 1 } ,
R _ {1 1} = 1
and, using the relationships above, we obtain
R _ {2 2} = \sqrt {\frac {r _ {y} (r _ {x} + 1)}{r _ {x} (r _ {y} + 1)}}, \qquad R _ {3 3} = \sqrt {\frac {r _ {y} (r _ {x} + 1)}{(r _ {x} + r _ {y})}}.
Again, if r _ { x } = r _ { y } = 1 , R _ { 2 2 } = R _ { 3 3 } = 1 and the Mises isotropic plasticity model is recovered.
General anisotropy
Thus far, we have only considered loading applied along the axes of anisotropy. To derive a more general anisotropic model in plane stress, the sheet must be loaded in one other direction in its plane. Suppose we perform a simple tension test at an angle to the x-direction; then, from equilibrium considerations we can write the nonzero stress components as
\sigma_ {1 1} = \sigma \cos^ {2} \alpha , \quad \sigma_ {2 2} = \sigma \sin^ {2} \alpha , \quad \sigma_ {1 2} = \sigma \sin \alpha \cos \alpha ,
where \sigma is the applied tensile stress. Substituting these values in the flow equations and assuming small elastic strains yields
d \varepsilon_ {1 1} = [ (G + H) \cos^ {2} \alpha - H \sin^ {2} \alpha ] \frac {\sigma}{f} d \lambda ,
\begin{array}{l} d \varepsilon_ {2 2} = [ (F + H) \sin^ {2} \alpha - H \cos^ {2} \alpha ] \frac {\sigma}{f} d \lambda , \\ d \varepsilon_ {3 3} = - \left[ F \sin^ {2} \alpha + G \cos^ {2} \alpha \right] \frac {\sigma}{f} d \lambda , \text { and } \\ d \gamma_ {1 2} = [ N \sin \alpha \cos \alpha ] \frac {\sigma}{f} d \lambda . \\ \end{array}
Assuming small geometrical changes, the width strain increment (the increment of strain at right angles to the direction of loading, ) is written as
d \varepsilon_ {\alpha + \frac {\pi}{2}} = d \varepsilon_ {1 1} \sin^ {2} \alpha + d \varepsilon_ {2 2} \cos^ {2} \alpha - 2 d \gamma_ {1 2} \sin \alpha \cos \alpha ,
and Lankford’s r-value for loading at an angle is
r _ {\alpha} = \frac {d \varepsilon_ {\alpha + \frac {\pi}{2}}}{d \varepsilon_ {3 3}} = \frac {H + (2 N - F - G - 4 H) \sin^ {2} \alpha \cos^ {2} \alpha}{F \sin^ {2} \alpha + G \cos^ {2} \alpha}.
One of the more commonly performed tests is that in which the loading direction is at 4 5 ^ { \circ } . In this case
r _ {4 5} = \frac {2 N - (F + G)}{2 (F + G)} \quad \mathrm{or} \quad \frac {N}{G} = (r _ {4 5} + \frac {1}{2}) (1 + \frac {r _ {x}}{r _ {y}}).
If \sigma ^ { 0 } is equal to \bar { \sigma } _ { 1 1 } in the metal plasticity model, R _ { 1 1 } = 1 . \ R _ { 2 2 } , R _ { 3 3 } are as defined before for transverse or planar anisotropy and, using the relationships above,
R _ {1 2} = \sqrt {\frac {3 (r _ {x} + 1) r _ {y}}{(2 r _ {4 5} + 1) (r _ {x} + r _ {y})}}.
Progressive damage and failure
In Abaqus/Explicit anisotropic yield can be used in conjunction with the models of progressive damage and failure discussed in “Damage and failure for ductile metals: overview,” Section 24.2.1. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), and Müschenborn-Sonne forming limit diagram (MSFLD) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The model offers two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations.
Input File Usage: Use the following options:
*PLASTIC
*DAMAGE INITIATION
*DAMAGE EVOLUTION
| Abaqus/CAE Usage: | Property module: material editor: Mechanical→Damage for DuctileMetals→damage initiation type: specify the damage initiation criterion:Suboptions→Damage Evolution: specify the damage evolution parameters |
Initial conditions
When we need to study the behavior of a material that has already been subjected to some work hardening, Abaqus allows you to prescribe initial conditions for the equivalent plastic strain, , by specifying the conditions directly (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).
Input File Usage: *INITIAL CONDITIONS, TYPE=HARDENING
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step
User subroutine specification in Abaqus/Standard
For more complicated cases, initial conditions can be defined in Abaqus/Standard through user subroutine HARDINI.
Input File Usage: *INITIAL CONDITIONS, TYPE=HARDENING, USER
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
Elements
Anisotropic yield can be defined for any element that can be used with the classical metal plasticity models in Abaqus (“Classical metal plasticity,” Section 23.2.1) except one-dimensional elements in Abaqus/Explicit (beams and trusses). In Abaqus/Standard it can also be defined for any element that can be used with the linear kinematic hardening plasticity model (“Models for metals subjected to cyclic loading,” Section 23.2.2) but not with the nonlinear isotropic/kinematic hardening model. Likewise, anisotropic creep can be defined for any element that can be used with the classical metal creep model in Abaqus/Standard (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4).
Output
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) and all output variables associated with the creep model (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4), classical metal plasticity models (“Classical metal plasticity,” Section 23.2.1), and the linear kinematic hardening plasticity model (“Models for metals subjected to cyclic loading,” Section 23.2.2) are available when anisotropic yield and creep are defined.
The following variables have special meaning if anisotropic yield and creep are defined:
PEEQ Equivalent plastic strain, \begin{array} { r } { \bar { \varepsilon } ^ { p l } = \bar { \varepsilon } ^ { p l } | _ { 0 } + \int _ { 0 } ^ { t } \dot { \bar { \varepsilon } } ^ { p l } d t = \bar { \varepsilon } ^ { p l } | _ { 0 } + \int _ { 0 } ^ { t } \frac { \sigma ; \dot { \varepsilon } ^ { p l } d t } { \sigma ^ { 0 } } } \end{array} g0 where \bar { \varepsilon } ^ { p l } | _ { 0 } is the initial equivalent plastic strain (zero or user-specified; see “Initial conditions”).
CEEQ Equivalent creep strain, \begin{array} { r } { \bar { \varepsilon } ^ { c r } = \int _ { 0 } ^ { t } \dot { \bar { \varepsilon } } ^ { c r } d t = \int _ { 0 } ^ { t } \frac { \pmb { \sigma } : \dot { \varepsilon } ^ { c r } d t } { \sigma ^ { 0 } } } \end{array} g0
YIELDS Yield stress, \sigma ^ { 0 }
23.2.7 JOHNSON-COOK PLASTICITY
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Classical metal plasticity,” Section 23.2.1
• “Rate-dependent yield,” Section 23.2.3
• “Equation of state,” Section 25.2.1
• Chapter 24, “Progressive Damage and Failure”
• “Dynamic failure models,” Section 23.2.8
• “Annealing or melting,” Section 23.2.5
• “Material library: overview,” Section 21.1.1
• “Inelastic behavior,” Section 23.1.1
• *ANNEAL TEMPERATURE
• *PLASTIC
• *RATE DEPENDENT
• *SHEAR FAILURE
• *TENSILE FAILURE
• *DAMAGE INITIATION
• *DAMAGE EVOLUTION
• “Using the Johnson-Cook hardening model to define classical metal plasticity” in “Defining plasticity,” Section 12.9.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
The Johnson-Cook plasticity model:
• is a particular type of Mises plasticity model with analytical forms of the hardening law and rate dependence;
• is suitable for high-strain-rate deformation of many materials, including most metals;
• is typically used in adiabatic transient dynamic simulations;
• can be used in conjunction with the Johnson-Cook dynamic failure model in Abaqus/Explicit;
• can be used in conjunction with the tensile failure model to model tensile spall or a pressure cutoff in Abaqus/Explicit;
• can be used in conjunction with the progressive damage and failure models (Chapter 24, “Progressive Damage and Failure”) to specify different damage initiation criteria and damage evolution laws that allow for the progressive degradation of the material stiffness and the removal of elements from the mesh; and
• must be used in conjunction with either the linear elastic material model (“Linear elastic behavior,” Section 22.2.1) or the equation of state material model (“Equation of state,” Section 25.2.1).
Yield surface and flow rule
A Mises yield surface with associated flow is used in the Johnson-Cook plasticity model.
Johnson-Cook hardening
Johnson-Cook hardening is a particular type of isotropic hardening where the static yield stress, \sigma ^ { 0 } , is assumed to be of the form
\sigma^ {0} = \Big [ A + B \big (\bar {\varepsilon} ^ {p l} \big) ^ {n} \Big ] \Big (1 - \hat {\theta} ^ {m} \Big),
where \bar { \varepsilon } ^ { p l } is the equivalent plastic strain and A, B, n and m are material parameters measured at or below the transition temperature, \theta _ { \mathrm { t r a n s i t i o n } } . is the nondimensional temperature defined as
\hat {\theta} \equiv \left\{ \begin{array}{c c c} 0 & \mathrm{for} & \theta < \theta_ {\mathrm{transition}} \\ (\theta - \theta_ {\mathrm{transition}}) / (\theta_ {\mathrm{melt}} - \theta_ {\mathrm{transition}}) & \mathrm{for} & \theta_ {\mathrm{transition}} \leq \theta \leq \theta_ {\mathrm{melt}} \\ 1 & \mathrm{for} & \theta > \theta_ {\mathrm{melt}} \end{array} \right.,
where is the current temperature, \theta _ { \mathrm { m e l t } } is the melting temperature, and \theta _ { \mathrm { t r a n s i t i o n } } is the transition temperature defined as the one at or below which there is no temperature dependence of the yield stress. The material parameters must be measured at or below the transition temperature.
When \theta \geq \theta _ { \mathrm { m e l t } } , the material will be melted and will behave like a fluid; there will be no shear resistance since \sigma ^ { 0 } = 0 . The hardening memory will be removed by setting the equivalent plastic strain to zero. If backstresses are specified for the model, these will also be set to zero.
If you include annealing behavior in the material definition and the annealing temperature is defined to be less than the melting temperature specified for the metal plasticity model, the hardening memory will be removed at the annealing temperature and the melting temperature will be used strictly to define the hardening function. Otherwise, the hardening memory will be removed automatically at the melting temperature. If the temperature of the material point falls below the annealing temperature at a subsequent point in time, the material point can work harden again. For more details, see “Annealing or melting,” Section 23.2.5.
You provide the values of A, B, n, m, \theta _ { \mathrm { m e l t } } , and \theta _ { \mathrm { t r a n s i t i o n } } as part of the metal plasticity material definition.
Input File Usage: *PLASTIC, HARDENING=JOHNSON COOK
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook
Johnson-Cook strain rate dependence
Johnson-Cook strain rate dependence assumes that
\bar {\sigma} = \sigma^ {0} (\bar {\varepsilon} ^ {p l}, \theta) R (\dot {\bar {\varepsilon}} ^ {p l})
and
\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
| $\bar{\sigma}$ | is the yield stress at nonzero strain rate; |
| $\dot{\bar{\varepsilon}}^{pl}$ | is the equivalent plastic strain rate; |
| $\dot{\varepsilon}_{0}$ and $C$ | are material parameters measured at or below the transition temperature, $\theta_{\text{transition}}$ ; |
| $\sigma^{0}(\bar{\varepsilon}^{pl}, \theta)$ | is the static yield stress; and |
| $R(\dot{\bar{\varepsilon}}^{pl})$ | is the ratio of the yield stress at nonzero strain rate to the static yield stress (so that $R(\dot{\varepsilon}_{0}) = 1.0$ ). |
The yield stress is, therefore, expressed as
\bar {\sigma} = \Big [ A + B \big (\bar {\varepsilon} ^ {p l} \big) ^ {n} \Big ] \Bigg [ 1 + C \ln \left(\frac {\dot {\bar {\varepsilon}} ^ {p l}}{\dot {\varepsilon} _ {0}}\right) \Bigg ] \Big (1 - \hat {\theta} ^ {m} \Big).
You provide the values of C and when you define Johnson-Cook rate dependence.
The use of Johnson-Cook hardening does not necessarily require the use of Johnson-Cook strain rate dependence.
Input File Usage: Use both of the following options:
*PLASTIC, HARDENING=JOHNSON COOK*RATE DEPENDENT, TYPE=JOHNSON COOK
Abaqus/CAE Usage: Property module: material editor: Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook: Suboptions→Rate Dependent: Hardening: Johnson-Cook
Johnson-Cook dynamic failure
Abaqus/Explicit provides a dynamic failure model specifically for the Johnson-Cook plasticity model, which is suitable only for high-strain-rate deformation of metals. This model is referred to as the “Johnson-Cook dynamic failure model.” Abaqus/Explicit also offers a more general implementation of the Johnson-Cook failure model as part of the family of damage initiation criteria, which is the recommended technique for modeling progressive damage and failure of materials (see “Damage and failure for ductile metals: overview,” Section 24.2.1). The Johnson-Cook dynamic failure model is based on the value of the equivalent plastic strain at element integration points; failure is assumed to occur when the damage parameter exceeds 1. The damage parameter, , is defined as
\omega = \sum \left(\frac {\Delta \bar {\varepsilon} ^ {p l}}{\bar {\varepsilon} _ {f} ^ {p l}}\right),
where \Delta \bar { \varepsilon } ^ { p l } is an increment of the equivalent plastic strain, \bar { \varepsilon } _ { f } ^ { p l } is the strain at failure, and the summation is performed over all increments in the analysis. The strain at failure, \bar { \varepsilon } _ { f } ^ { p l } , is assumed to be dependent on a nondimensional plastic strain rate, \dot { \bar { \varepsilon } } ^ { p l } / \dot { \varepsilon } _ { 0 } ; a dimensionless pressure-deviatoric stress ratio, p / q (where \pmb { p } is the pressure stress and \pmb q is the Mises stress); and the nondimensional temperature, { \hat { \theta } } , defined earlier in the Johnson-Cook hardening model. The dependencies are assumed to be separable and are of the form
\bar {\varepsilon} _ {f} ^ {p l} = \left[ d _ {1} + d _ {2} \mathrm{exp} \left(d _ {3} \frac {p}{q}\right) \right] \left[ 1 + d _ {4} \mathrm{ln} \left(\frac {\dot {\bar {\varepsilon}} ^ {p l}}{\dot {\bar {\varepsilon}} _ {0}}\right) \right] \left(1 + d _ {5} \hat {\theta}\right),
where d _ { 1 } { - } d _ { 5 } are failure parameters measured at or below the transition temperature, \theta _ { \mathrm { t r a n s i t i o n } } , , and \dot { \varepsilon } _ { 0 } is the reference strain rate. You provide the values of d _ { 1 } { - } d _ { 5 } when you define the Johnson-Cook dynamic failure model. This expression for \bar { \varepsilon } _ { f } ^ { p l } differs from the original formula published by Johnson and Cook (1985) in the sign of the parameter d _ { 3 } . This difference is motivated by the fact that most materials experience an increase in \bar { \varepsilon } _ { f } ^ { p l } with increasing pressure-deviatoric stress ratio; therefore, d _ { 3 } in the above expression will usually take positive values.
When this failure criterion is met, the deviatoric stress components are set to zero and remain zero for the rest of the analysis. Depending on your choice, the pressure stress may also be set to zero for the rest of calculation (if this is the case, you must specify element deletion and the element will be deleted) or it may be required to remain compressive for the rest of the calculation (if this is the case, you must choose not to use element deletion). By default, the elements that meet the failure criterion are deleted.
The Johnson-Cook dynamic failure model is suitable for high-strain-rate deformation of metals; therefore, it is most applicable to truly dynamic situations. For quasi-static problems that require element removal, the progressive damage and failure models (Chapter 24, “Progressive Damage and Failure”) or the Gurson metal plasticity model (“Porous metal plasticity,” Section 23.2.9) are recommended.
The use of the Johnson-Cook dynamic failure model requires the use of Johnson-Cook hardening but does not necessarily require the use of Johnson-Cook strain rate dependence. However, the ratedependent term in the Johnson-Cook dynamic failure criterion will be included only if Johnson-Cook strain rate dependence is defined. The Johnson-Cook damage initiation criterion described in “Damage initiation for ductile metals,” Section 24.2.2, does not have these limitations.
Input File Usage: Use both of the following options:
*PLASTIC, HARDENING=JOHNSON COOK
*SHEAR FAILURE, TYPE=JOHNSON COOK,
ELEMENT DELETION=YES or NO
Abaqus/CAE Usage: Johnson-Cook dynamic failure is not supported in Abaqus/CAE.
Progressive damage and failure
The Johnson-Cook plasticity model can be used in conjunction with the progressive damage and failure models discussed in “Damage and failure for ductile metals: overview,” Section 24.2.1. The capability allows for the specification of one or more damage initiation criteria, including ductile, shear, forming limit diagram (FLD), forming limit stress diagram (FLSD), Müschenborn-Sonne forming limit diagram (MSFLD), and, in Abaqus/Explicit, Marciniak-Kuczynski (M-K) criteria. After damage initiation, the material stiffness is degraded progressively according to the specified damage evolution response. The models offer two failure choices, including the removal of elements from the mesh as a result of tearing or ripping of the structure. The progressive damage models allow for a smooth degradation of the material stiffness, making them suitable for both quasi-static and dynamic situations. This is a great advantage over the dynamic failure models discussed above.
Input File Usage: Use the following options:
*PLASTIC, HARDENING=JOHNSON COOK
*DAMAGE INITIATION
*DAMAGE EVOLUTION
Abaqus/CAE Usage: Property module: material editor: Mechanical→Damage for Ductile
Metals→damage initiation type: specify the damage initiation criterion:
Suboptions→Damage Evolution: specify the damage evolution parameters
Tensile failure
In Abaqus/Explicit the tensile failure model can be used in conjunction with the Johnson-Cook plasticity model to define tensile failure of the material. The tensile failure model uses the hydrostatic pressure stress as a failure measure to model dynamic spall or a pressure cutoff and offers a number of failure choices including element removal. Similar to the Johnson-Cook dynamic failure model, the Abaqus/Explicit tensile failure model is suitable for high-strain-rate deformation of metals and is most applicable to truly dynamic problems. For more details, see “Dynamic failure models,” Section 23.2.8.
Input File Usage: Use both of the following options:
*PLASTIC, HARDENING=JOHNSON COOK
*TENSILE FAILURE
Abaqus/CAE Usage: The tensile failure model is not supported in Abaqus/CAE.
Heat generation by plastic work
Abaqus allows for an adiabatic thermal-stress analysis (“Adiabatic analysis,” Section 6.5.4), a fully coupled temperature-displacement analysis (“Fully coupled thermal-stress analysis,” Section 6.5.3), or a fully coupled thermal-electrical-structural analysis (“Fully coupled thermal-electrical-structural analysis,” Section 6.7.4) to be performed in which heat generated by plastic straining of a material is calculated. This method is typically used in the simulation of bulk metal forming or high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material
caused by its deformation is an important effect because of temperature dependence of the material properties. Since the Johnson-Cook plasticity model is motivated by high-strain-rate transient dynamic applications, temperature change in this model is generally computed by assuming adiabatic conditions (no heat transfer between elements). Heat is generated in an element by plastic work, and the resulting temperature rise is computed using the specific heat of the material.
This effect is introduced by defining the fraction of the rate of inelastic dissipation that appears as a heat flux per volume.
Input File Usage: Use all of the following options in the same material data block:
*PLASTIC, HARDENING=JOHNSON COOK
*SPECIFIC HEAT
*DENSITY
*INELASTIC HEAT FRACTION
Abaqus/CAE Usage: Use all of the following options in the same material definition:
Property module: material editor:
Mechanical→Plasticity→Plastic: Hardening: Johnson-Cook
Thermal→Specific Heat
General→Density
Thermal→Inelastic Heat Fraction
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 “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). An initial backstress, \alpha _ { 0 } , can also be specified. The backstress \alpha _ { 0 } represents a constant kinematic shift of the yield surface, which can be useful for modeling the effects of residual stresses without considering them in the equilibrium solution.
Input File Usage: *INITIAL CONDITIONS, TYPE=HARDENING
Abaqus/CAE Usage: Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step
Elements
The Johnson-Cook plasticity model can be used with any elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom).
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 Johnson-Cook plasticity model: