Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
is intended to model the effects of melting and resolidification in metals subjected to high-temperature processes or the effects of annealing at a material point when its temperature rises above a certain level;
is available for only the Mises, Johnson-Cook, and Hill plasticity models;
is intended to be used in conjunction with appropriate temperature-dependent material properties (in particular, the model assumes perfectly plastic behavior at or above the annealing or melting temperature); and
can be modeled simply by defining an annealing or melting temperature.
When the temperature of a material point exceeds a user-specified value called the annealing temperature, ABAQUS assumes that the material point loses its hardening memory. The effect of prior work hardening is removed by setting the equivalent plastic strain to zero. For kinematic and combined hardening models the backstress tensor is also reset to zero. 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. Depending on the temperature history a material point may lose and accumulate memory several times, which in the context of modeling melting would correspond to repeated melting and resolidification. Any accumulated material damage is not healed when the annealing temperature is reached. Damage will continue to accumulate after annealing according to any damage model in effect (see Damage and failure for ductile metals: overview, Section 19.2.1).
In ABAQUS/Explicit an annealing step can be defined to simulate the annealing process for the entire model, independent of temperature; see Annealing procedure, Section 6.11.1, for details.
The annealing temperature is a material property that can optionally be defined as a function of field variables. This material property must be used in conjunction with an appropriate definition of material properties as functions of temperature for the Mises plasticity model. In particular, it is necessary that the hardening behavior be defined as a function of temperature, which is done by defining several yield stress versus plastic strain curves (each at a different temperature) for the plasticity model (see Classical metal plasticity, Section 18.2.1). For metals the yield stress typically decreases with increasing temperature. ABAQUS expects the hardening to vanish at or above the annealing temperature and will issue an error message if you specify otherwise in the material definition. Zero hardening may be specified by simply specifying a single data point (at zero plastic strain) in the yield stress versus plastic strain curve.
For hardening defined in ABAQUS/Standard with user subroutine UHARD, ABAQUS/Standard will check the hardening slope at or above the annealing temperature during the actual computations and will issue an error message if appropriate.
The Johnson-Cook plasticity model in ABAQUS/Explicit requires a separate melting temperature to define the hardening behavior. If 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.
|Input File Usage:|
Property module: material editor: MechanicalPlasticityPlastic: SuboptionsAnneal Temperature
The following input is an example of a typical usage of the annealing or melting capability. It is assumed that you have defined the stress versus plastic strain behavior (see Figure 18.2.51) for the isotropic hardening model at three different temperatures, including the annealing temperature.
This capability can be used with all elements that include mechanical behavior (elements that have displacement degrees of freedom).
Only the equivalent plastic strain (output variable PEEQ) and the backstress (output variable ALPHA) are reset to zero at the melting temperature. The plastic strain tensor (output variable PE) is not reset to zero and provides a measure of the total plastic deformation during the analysis. In ABAQUS/Standard the plastic strain tensor also provides a measure of the plastic strain magnitude (output variable PEMAG).