Annealing

The anneal procedure:

is used to anneal a structure by setting all appropriate state variables and velocities to zero;
is intended for metal plasticity and user-defined material models; and
can also be used with linear elastic materials and with superelastic materials for modeling shape setting in Abaqus/Explicit.

It has no effect on other material models.

This page discusses:

The Annealing Process
Initial Conditions
Boundary Conditions
Loads
Predefined Fields
Material Options
Elements
Output
Input File Template

The Annealing Process

The anneal procedure is intended to simulate the relaxation of stresses and plastic strains that occurs as metals are heated to high temperatures. Physically, annealing is the process of heating a metal part to a high temperature to allow the microstructure to recrystallize, removing dislocations caused by cold working of the material. During the anneal procedure, Abaqus/Explicit sets all appropriate state variables to zero. These variables include stresses, backstresses, plastic strains, and velocities. In the case of metal porous plasticity, the void volume fraction is also set to zero, such that the material becomes fully dense.

There is no time scale in an annealing step; therefore, time does not advance. The annealing process occurs instantaneously. No data are required for the anneal procedure.

Input File Usage

          
            ANNEAL

Abaqus/CAE Usage

Step module: Create Step: General: Anneal

Temperatures

Thermal strains are set to zero, and the temperature at all nodes in the model will be set to a uniform temperature or will be maintained at the current temperature during the anneal procedure. By default, the temperature at all nodes is maintained at the current temperature. You can specify a different final temperature, $θ$ .

Input File Usage

ANNEAL, TEMPERATURE= $θ$

Abaqus/CAE Usage

Step module: Create Step: General: Anneal: Post-anneal reference temperature: Value  $θ$

Initial Conditions

The initial state for the anneal step is the state of the model at the end of the last explicit dynamic analysis step.

Boundary Conditions

It is not appropriate to specify new boundary conditions or to modify boundary conditions in an anneal procedure; all boundary conditions in effect prior to this procedure will remain fixed.

Loads

It is not meaningful to specify loads in an anneal procedure.

Predefined Fields

It is not meaningful to specify predefined fields in an anneal procedure.

Material Options

The annealing procedure is intended for metal plasticity models (Classical Metal Plasticity) and user-defined materials modeled with user subroutines VFABRIC and VUMAT. The metal plasticity models in Abaqus/Explicit include Mises, Johnson-Cook, Hill, and metal porous plasticity. Abaqus/Explicit also allows annealing of linear elastic materials (Linear Elastic Behavior, including isotropic, orthotropic, and anisotropic elasticity), as well as annealing of superelastic materials for modeling shape setting (Superelasticity). The annealing procedure has no effect on other material models.

Elements

All of the elements that are available in Abaqus/Explicit can be used in an anneal procedure. The elements are listed in Abaqus Elements Guide.

Output

There is no output associated with an anneal step.

Input File Template

HEADING
 …
**
STEP
DYNAMIC, EXPLICIT (,ADIABATIC) or 
DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT
Data line to specify the time period of the step
BOUNDARY, AMPLITUDE=name
Data lines to describe zero-valued or nonzero boundary conditions
CLOAD and/or DLOAD
Data lines to specify loads
TEMPERATURE and/or FIELD
Data lines to specify values of predefined fields
END STEP
**
STEP
ANNEAL (,TEMPERATURE= $θ$ )
END STEP
**
STEP
DYNAMIC, EXPLICIT (,ADIABATIC)
Data line to specify the time period of the step
BOUNDARY, AMPLITUDE=name
Data lines to describe zero-valued or nonzero boundary conditions
CLOAD and/or DLOAD and/or DSLOAD
Data lines to specify loads
TEMPERATURE and/or FIELD
Data lines to specify values of predefined fields
END STEP