Mechanical APDL Basic Analysis Guide

4.2.5. Initial State with State Variables Application

To use the initial state capability with state variables via the INISTATE command, simply change the
data type to SVAR, as shown:

! Apply initial state – state variables.

! This fictitious svar example contains 7 components:

! The 1st component is accumulated equivalent plastic strain.

! Components 2-7 are plastic strains values.

! at all the selected elements

inistate,set,dtyp,svar

inistate,defi,,,,,0.005,0.1,-0.02,0.02,0,0,0

The INISTATE command does not consider the coordinate systems of quantities stored within the state
variables. It is therefore your responsibility to account for the transformations.

For an initial state example problem that uses state variables, see Example: Initial Plastic Strain Problem
Using the INISTATE with State Variables (p. 105).

4.2.6. Node-Based Initial Strain Application

As shown below, a node-based initial state can be applied to all nodes or to a selected subset of nodes.
Layer numbers can also be specified.

! Enable Node-Based Initial State

inis,set,node,1

! Apply elastic strains at all nodes in layer 1 and 3

inistate,set,dtyp,epel

inistate,defi,all,,1,,0.005

inistate,defi,all,,3,,0.005

! Apply a different elastic strain at all nodes in layer 2

inistate,defi,all,,2,,0.010

! Apply zero elastic strain at node 10

inistate,defi,10,,all,,0.000

! Apply zero elastic strain at node selection

nsel,s,loc,x,0

inistate,defi,all,,all,,0.000

For a node-based initial state example problem, see Example: Node-Based Initial Strain Problem Using
the INISTATE Command (p. 107).

4.3. Initial State File Format

Although you can use the INISTATE command repeatedly to assign explicit values to various items,
creating an external file simplifies the process.

You can create a standalone initial state file to be read into your analysis via an INISTATE,READ command.
The file format must be comma-delimited ASCII, consisting of individual rows for each stress item. Each
of the rows consists of columns separat ed by commas. Your columns delineate the integration point(s)
for the specific elements.

See Integration Point Locations in the Mechanical APDL Theory Reference for more information about
the number and location of available element integration points. Also see Element Library in the
Mechanical APDL Theory Reference for a listing of the integration points for each specific element.

The number of section integration points for beams and cells is dependent upon the associated user
input. One element ID number can be repeated on successive lines to specify different stresses at dif-
ferent integration points.

Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information

Initial State File Format