Mechanical APDL Basic Analysis Guide - Ansys

Chapter 4: Initial State
! Apply a Strain of EPEL X=0.01 at Elem Integration Pt 3 within Element 2.
! Here it is assumed that the initial stress is zero.
inis,set,dtyp,eppl
inis,defi,2,3,,,0.01
! Apply accumulated equivalent plastic strain.
inis,set,dtyp,pleq
inis,defi,2,3,,,0.02
! Apply EPS X = 0.1, EPS Y = -0.02, EPS Z = -0.02, for Layers 1,3,5 and
! EPS X = 0.2, for Layers 2,4,6
! Layer 1,3,5 have material 1 and Layer 2,4,6 have material 2.
inis,set,dtype,eppl
inis,set,mat,1
inis,defi,,,,,2.0
inis,set,mat,2
inis,defi,,,,,0.2
For an initial plastic strain example problem, see Example: Initial Plastic Strain Problem Using the INISTATE
Command (p. 94).
4.4. 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 separated by commas. Your columns delineate the integration point(s) for the
specific elements.
See Integration Point Locations in the Theory Reference for the Mechanical APDL and Mechanical Applications
for more information about the number and location of available element integration points. Also see "Element
Library" in the Theory Reference for the Mechanical APDL and Mechanical Applications 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 different integration
points.
Each line of the initial stress file has 10 columns, as follows:
• The element ID Number
• The element integration point (for standard elements)
• The layer (for layered elements) or the cell number (for beams)
• The section integration point (for beams and shells only)
• The six stress/strain components
Any of the parameters for element ID, element integration point, layer number, cell number, or section integration
point can be set to ALL. For example,
1,all,all,all, 100, 0, 0, 0, 0, 0
applies an equal stress of SX = 100 to all integration points or layers of the element ID = 1.
This input line
90
all,all,all,all, 100, 0, 0, 0, 0, 0
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.