ORNL – Oak Ridge National Laboratory constitutive model | ||
| ||
ProductsAbaqus/StandardAbaqus/CAE
Usage with plasticity
The ORNL constitutive model in Abaqus/Standard is based on the March 1981 issue of the Nuclear Standard NEF 9–5T and on the October 1986 issue, which revises the constitutive model extensively. This model adds isotropic hardening of the plastic yield surface from a virgin material state to a fully cycled state. Initially the material is assumed to harden kinematically according to a bilinear representation of the virgin stress-strain curve. If a strain reversal takes place or if the creep strain reaches 0.2%, the yield surface expands isotropically to the user-defined tenth-cycle stress-strain curve. Further hardening occurs kinematically according to a bilinear representation of the tenth-cycle stress-strain curve.
You must specify the virgin yield stress and the hardening through a plasticity model definition and the elastic part of the response through a linear elasticity model definition. You specify the tenth-cycle yield stress and hardening values separately. The yield stress at each temperature should be defined by giving its value at zero plastic strain and at one additional nonzero plastic strain point, thus giving a constant hardening rate (linear work hardening).
Input File Usage
Use all of the following options in the same material data block:
PLASTIC ORNL CYCLED PLASTIC
Abaqus/CAE Usage
Property module: material editor: : and
Abaqus/Standard also allows you to invoke the optional kinematic shift () reset procedure that is described in Section 4.3.5 of the Nuclear Standard. If you do not specify the reset procedure explicitly, it is not used.
Input File Usage
ORNL, RESET
Abaqus/CAE Usage
Property module: material editor: : Invoke reset procedure
Usage with creep
The ORNL constitutive model assumes that creep uses the strain hardening formulation. It introduces auxiliary hardening rules when strain reversals occur. An algorithm providing details is presented in ORNL constitutive theory. It can be used only when the creep behavior is defined by a strain-hardening power law.
Input File Usage
Use both of the following options in the same material data block:
CREEP, LAW=STRAIN ORNL
Abaqus/CAE Usage
Property module: material editor: : Law: Strain-Hardening:
Translation of the yield surface during creep
The ORNL formulation can also cause the center of the yield surface to translate during creep for use in subsequent plastic increments; this behavior is defined through two optional user-defined parameters.
Specifying saturation rates for kinematic shift
You can specify A, the saturation rates for kinematic shift caused by creep strain as defined by Equation (15) of Section 4.3.3–3 of the Nuclear Standard. The default value is 0.3. Set A=0.0 to use the 1986 revision of the standard.
Input File Usage
ORNL, A=A
Abaqus/CAE Usage
Property module: material editor: : Saturation rates for kinematic shift: A
Specifying the rate of kinematic shift
You can specify H, the rate of kinematic shift with respect to creep strain (Equation (7) of Section 4.3.2–1 of the Nuclear Standard). Set H=0.0 to use the 1986 revision of the standard. If you do not specify a value for H, it is determined according to Section 4.3.3–3 of the 1981 revision of the standard.
Input File Usage
ORNL, H=H
Abaqus/CAE Usage
Property module: material editor: : Rate of kinematic shift wrt creep strain: H
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 Inelastic behavior for additional details. Initial values can also be provided for the backstress tensor, , to include strain-induced anisotropy. See Initial conditions in Abaqus/Standard and Abaqus/Explicit for more information. For more complicated cases initial conditions can be defined through user subroutine HARDINI.
Input File Usage
Use the following option to specify the initial equivalent plastic strain directly:
INITIAL CONDITIONS, TYPE=HARDENING
Use the following option in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI:
INITIAL CONDITIONS, TYPE=HARDENING, USER
Abaqus/CAE Usage
Use the following options to specify the initial equivalent plastic strain directly:
Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step
Use the following options in Abaqus/Standard to specify the initial equivalent plastic strain in user subroutine HARDINI:
Load module: Create Predefined Field: Step: Initial, choose Mechanical for the Category and Hardening for the Types for Selected Step; Definition: User-defined
Elements
The ORNL constitutive model can be used with any elements in Abaqus/Standard that include mechanical behavior (elements that have displacement degrees of freedom).
Output
In addition to the standard output identifiers available in Abaqus/Standard (Abaqus/Standard output variable identifiers), variables associated with creep (Rate-dependent plasticity: creep and swelling) and the kinematic hardening plasticity models (Models for metals subjected to cyclic loading) are available for the ORNL constitutive model.