Mechanical APDL Basic Analysis Guide - Ansys

Chapter 4: Initial State
/CSYS,0
! ELEM ID ELEM INTG LAY/CELL SECT INTG SX SY SZ SXY SYZ SXZ
1 , 1, , , 100, 0, 0, 0, 0, 0
1 , 2, , , 100, 0, 0, 0, 0, 0
1 , 3, , , 100, 0, 0, 0, 0, 0
1 , 4, , , 100, 0, 0, 0, 0, 0
1 , 5, , , 100, 0, 0, 0, 0, 0
1 , 6, , , 100, 0, 0, 0, 0, 0
1 , 7, , , 100, 0, 0, 0, 0, 0
1 , 8, , , 100, 0, 0, 0, 0, 0
In the following input listing, initial stress loading data is read in from a file. The data is read in during the
first load step, and establishes a preliminary deflection corresponding to a tip loaded cantilever beam with
a tip load of 1e5 units.
/prep7
/title, Example of Initial stress import into ANSYS
et,1,182
! Plane stress PLANE182 element
mp,ex,1,1.0e9
mp,nuxy,1,0.3
!
! Define the nodes
!
n,1
n,2,2.0
n,3,4.0
n,4,6.0
n,5,8.0
n,6,10.0
n,7,,1.0
n,8,2.0,1.0
n,9,4.0,1.0
n,10,6.0,1.0
n,11,8.0,1.0
n,12,10.0,1.0
!
! Define the 5 elements
!
e,1,2,8,7
e,2,3,9,8
e,3,4,10,9
e,4,5,11,10
e,5,6,12,11
! Constrain all dofs on all nodes at x=0 to be zero
nsel,s,loc,x,
d,all,all
nall
finish
!
/solu
! Read in the initial stresses from istress.ist file
! as loading in the 1st load step.
! Input stresses correspond to the element integration
! point location.
!
inis,read,istress,ist
! List the initial stresses
inis,list
outres,all,all
solve
finish
!
/post1
set,last
prnsol,u
finish
The INISTATE,WRITE command specifies the coordinate system into which the data is to be written.
92
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.