You can create a hardening field to define initial values of state variables for plastic hardening. For more information, see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1 of the Abaqus Analysis User's Guide.
To create or edit a hardening field:
Display the hardening field editor using one of the following methods:
To create a new hardening field, follow the procedure outlined in “Creating predefined fields,” Section 16.8.3 (Category: Mechanical; Types for Selected Step: Hardening).
To edit an existing hardening field using menus or managers, see “Editing step-dependent objects,” Section 3.4.13.
Note: You can create or edit a hardening field only in the initial step.
Click the arrow to the right of the Distribution field, and select the option of your choice from the list that appears:
Select Uniform to define initial values that are uniform over the region.
Select an analytical field to define spatially varying initial values. Alternatively, you can click 
to create a new analytical field. (See Chapter 58, “The Analytical Field toolset,” for more information.)
Click the arrow to the right of the Definition field, and select the option of your choice from the list that appears:
Select Kinematic hardening to specify an initial equivalent plastic strain and the initial backstress tensors for kinematic hardening material models.
Select Crushable foam to specify an initial volumetric compacting plastic strain for the crushable foam material model.
Select Rebar to specify an initial equivalent plastic strain and the initial backstress tensors for rebar layers. (This option is valid only for Abaqus/Standard analyses.)
Select Section points to specify an initial equivalent plastic strain and the initial backstress tensors at section points through the thickness of shell elements.
Select User-defined to specify the initial equivalent plastic strain and, if relevant, the initial backstress tensors in user subroutine HARDINI. (This option is valid only in Abaqus/Standard analyses.) See the following sections for more information:
If applicable, click the arrows to the right of the Number of backstresses field to specify the number of backstresses to include in the model. The default number of backstresses is 1. The maximum number of backstresses allowed is 10.
Additional columns appear in the Data table to specify multiple backstress tensors.
In the Data table, enter the data relevant to your Definition selection (not all of the following parameters will apply):
Equiv Plast Strain
Initial equivalent plastic strain, 
.
Vol Plast Strain
Initial volumetric compacting plastic strain, 
.
Rebar Layer Name
Name of rebar layer.
Section Point Number
Section point number.
Alpha 1_11, Alpha 1_22, etc.
Values for each component of the initial first backstress tensor, 
.
Alpha k_11, Alpha k_22, etc.
Values for each component of the initial kth backstress tensor, 
.
Click OK to save your data and to exit the editor.
