ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE Yield surface and flow ruleA Mises yield surface with associated flow is used in the JohnsonCook plasticity model. JohnsonCook hardeningJohnsonCook hardening is a particular type of isotropic hardening where the static yield stress, ${\sigma}^{0}$, is assumed to be of the form $${\sigma}^{0}=\left[A+B{\left({\overline{\epsilon}}^{pl}\right)}^{n}\right]\left(1{\widehat{\theta}}^{m}\right),$$ where ${\overline{\epsilon}}^{pl}$ is the equivalent plastic strain and A, B, n and m are material parameters measured at or below the transition temperature, ${\theta}_{\mathrm{transition}}$. $\widehat{\theta}$ is the nondimensional temperature defined as $$\widehat{\theta}\equiv \{\begin{array}{cc}\hfill 0\hfill & \text{for}\theta {\theta}_{\mathrm{transition}}\hfill \\ \hfill \left(\theta {\theta}_{\mathrm{transition}}\right)/\left({\theta}_{\mathrm{melt}}{\theta}_{\mathrm{transition}}\right)\hfill & \text{for}{\theta}_{\mathrm{transition}}\le \theta \le {\theta}_{\mathrm{melt}}\hfill \\ \hfill 1\hfill & \text{for}\theta {\theta}_{\mathrm{melt}}\hfill \end{array},$$ where $\theta $ is the current temperature, ${\theta}_{\mathrm{melt}}$ is the melting temperature, and ${\theta}_{\mathrm{transition}}$ 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 $\theta \ge {\theta}_{\mathrm{melt}}$, 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. You provide the values of A, B, n, m, ${\theta}_{\mathrm{melt}}$, and ${\theta}_{\mathrm{transition}}$ as part of the metal plasticity material definition. Input File Usage PLASTIC, HARDENING=JOHNSON COOK Abaqus/CAE Usage Property module: material editor: MechanicalPlasticityPlastic: Hardening: JohnsonCook JohnsonCook strain rate dependenceJohnsonCook strain rate dependence assumes that $$\overline{\sigma}={\sigma}^{0}\left({\overline{\epsilon}}^{pl},\theta \right)R\left({\dot{\overline{\epsilon}}}^{pl}\right)$$ and $${\dot{\overline{\epsilon}}}^{pl}={\dot{\epsilon}}_{0}\mathrm{exp}\left[\frac{1}{C}\left(R1\right)\right]\text{for}\overline{\sigma}\ge {\sigma}^{0},$$ where
The yield stress is, therefore, expressed as $$\overline{\sigma}=\left[A+B{\left({\overline{\epsilon}}^{pl}\right)}^{n}\right]\left[1+C\text{\hspace{0.17em}}\text{\hspace{0.17em}}\text{\hspace{0.17em}}\mathrm{ln}\left(\frac{{\dot{\overline{\epsilon}}}^{pl}}{{\dot{\epsilon}}_{0}}\right)\right]\left(1{\widehat{\theta}}^{m}\right).$$ You provide the values of C and ${\dot{\epsilon}}_{0}$ when you define JohnsonCook rate dependence. The use of JohnsonCook hardening does not necessarily require the use of JohnsonCook 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: MechanicalPlasticityPlastic: Hardening: JohnsonCook: SuboptionsRate Dependent: Hardening: JohnsonCook JohnsonCook dynamic failureAbaqus/Explicit provides a dynamic failure model specifically for the JohnsonCook plasticity model, which is suitable only for highstrainrate deformation of metals. This model is referred to as the “JohnsonCook dynamic failure model.” Abaqus/Explicit also offers a more general implementation of the JohnsonCook 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 About damage and failure for ductile metals). The JohnsonCook 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, $\omega $, is defined as $$\omega =\sum \left(\frac{\mathrm{\Delta}{\overline{\epsilon}}^{pl}}{{\overline{\epsilon}}_{f}^{pl}}\right),$$ where $\mathrm{\Delta}{\overline{\epsilon}}^{pl}$ is an increment of the equivalent plastic strain, ${\overline{\epsilon}}_{f}^{pl}$ is the strain at failure, and the summation is performed over all increments in the analysis. The strain at failure, ${\overline{\epsilon}}_{f}^{pl}$, is assumed to be dependent on a nondimensional plastic strain rate, ${\dot{\overline{\epsilon}}}^{pl}/{\dot{\epsilon}}_{0}$; a dimensionless pressuredeviatoric stress ratio, $p/q$ (where p is the pressure stress and q is the Mises stress); and the nondimensional temperature, $\widehat{\theta}$, defined earlier in the JohnsonCook hardening model. The dependencies are assumed to be separable and are of the form $${\overline{\epsilon}}_{f}^{pl}=\left[{d}_{1}+{d}_{2}\mathrm{exp}\left({d}_{3}\frac{p}{q}\right)\right]\left[1+{d}_{4}\mathrm{ln}\left(\frac{{\dot{\overline{\epsilon}}}^{pl}}{{\dot{\epsilon}}_{0}}\right)\right]\left(1+{d}_{5}\widehat{\theta}\right),$$ where ${d}_{1}$–${d}_{5}$ are failure parameters measured at or below the transition temperature, ${\theta}_{\mathrm{transition}}$, and ${\dot{\epsilon}}_{0}$ is the reference strain rate. You provide the values of ${d}_{1}$–${d}_{5}$ when you define the JohnsonCook dynamic failure model. This expression for ${\overline{\epsilon}}_{f}^{pl}$ 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 ${\overline{\epsilon}}_{f}^{pl}$ with increasing pressuredeviatoric 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 JohnsonCook dynamic failure model is suitable for highstrainrate deformation of metals; therefore, it is most applicable to truly dynamic situations. For quasistatic problems that require element removal, the progressive damage and failure models (Progressive Damage and Failure) or the Gurson metal plasticity model (Porous metal plasticity) are recommended. The use of the JohnsonCook dynamic failure model requires the use of JohnsonCook hardening but does not necessarily require the use of JohnsonCook strain rate dependence. However, the ratedependent term in the JohnsonCook dynamic failure criterion will be included only if JohnsonCook strain rate dependence is defined. The JohnsonCook damage initiation criterion described in Damage initiation for ductile metals 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 JohnsonCook dynamic failure is not supported in Abaqus/CAE. Progressive damage and failureThe JohnsonCook plasticity model can be used in conjunction with the progressive damage and failure models discussed in About damage and failure for ductile metals. 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), MüschenbornSonne forming limit diagram (MSFLD), and, in Abaqus/Explicit, MarciniakKuczynski (MK) 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 quasistatic 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: MechanicalDamage for Ductile Metalsdamage initiation type: specify the damage initiation criterion: SuboptionsDamage Evolution: specify the damage evolution parameters Tensile failureIn Abaqus/Explicit the tensile failure model can be used in conjunction with the JohnsonCook 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 JohnsonCook dynamic failure model, the Abaqus/Explicit tensile failure model is suitable for highstrainrate deformation of metals and is most applicable to truly dynamic problems. For more details, see Dynamic failure models. Abaqus/CAE Usage The tensile failure model is not supported in Abaqus/CAE. Heat generation by plastic workAbaqus allows for an adiabatic thermalstress analysis (Adiabatic analysis), a fully coupled temperaturedisplacement analysis (Fully coupled thermalstress analysis), or a fully coupled thermalelectricalstructural analysis (Fully coupled thermalelectricalstructural analysis) 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 highspeed 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 JohnsonCook plasticity model is motivated by highstrainrate 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: MechanicalPlasticityPlastic: Hardening: JohnsonCook ThermalSpecific Heat GeneralDensity ThermalInelastic Heat Fraction Initial conditionsWhen 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). An initial backstress, ${\mathit{\alpha}}_{0}$, can also be specified. The backstress ${\mathit{\alpha}}_{0}$ 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 ElementsThe JohnsonCook plasticity model can be used with any elements in Abaqus that include mechanical behavior (elements that have displacement degrees of freedom). OutputIn addition to the standard output identifiers available in Abaqus (Abaqus/Standard output variable identifiers and Abaqus/Explicit output variable identifiers), the following variables have special meaning for the JohnsonCook plasticity model:
References
