Products: ABAQUS/Explicit ABAQUS/CAE
The anneal procedure:
is used to anneal a structure by setting all appropriate state variables and velocities to zero; and
is intended only for metal plasticity and user-defined material models; it has no effect on other material models.
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 |
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, 
.
| Input File Usage: | *ANNEAL, TEMPERATURE= |
| ABAQUS/CAE Usage: | Step module: Create Step: General: Anneal: Post-anneal reference temperature: Value |
The initial state for the anneal step is the state of the model at the end of the last explicit dynamic analysis step.
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.
The annealing procedure is intended only for metal plasticity models (“Classical metal plasticity,” Section 18.2.1) and user-defined materials modeled with user subroutine VUMAT. The metal plasticity models in ABAQUS/Explicit include Mises, Johnson-Cook, Hill, and metal porous plasticity. ABAQUS/Explicit also allows annealing of elastic materials (“Linear elastic behavior,” Section 17.2.1), including isotropic, orthotropic, and anisotropic elasticity. The annealing procedure has no effect on other material models.
All of the elements that are available in ABAQUS/Explicit can be used in an anneal procedure. The elements are listed in Part VI, “Elements.”
*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=