#

##

This tutorial was created using ANSYS 7.0
The purpose of this tutorial is to outline the steps required to view cross sectional results (Deformation, Stress, etc.) of the following example.

## ANSYS Command Listing

FINISH
/CLEAR
/Title, Cross-Sectional Results of a Simple Cantilever Beam
/PREP7
! All dims in mm
Width = 60
Height = 40
Length = 400
BLC4,0,0,Width,Height,Length ! Creates a rectangle
/ANGLE, 1 ,60.000000,YS,1 ! Rotates the display
/REPLOT,FAST ! Fast redisplay
ET,1,SOLID45 ! Element type
MP,EX,1,200000 ! Young's Modulus
MP,PRXY,1,0.3 ! Poisson's ratio
esize,20 ! Element size
vmesh,all ! Mesh the volume
FINISH
/SOLU ! Enter solution mode
ANTYPE,0 ! Static analysis
ASEL,S,LOC,Z,0 ! Area select at z=0
DA,All,ALL,0 ! Constrain the area
ASEL,ALL ! Reselect all areas
KSEL,S,LOC,Z,Length ! Select certain keypoint
KSEL,R,LOC,Y,Height
KSEL,R,LOC,X,Width
FK,All,FY,-2500 ! Force on keypoint
KSEL,ALL ! Reselect all keypoints
SOLVE ! Solve
FINISH
/POST1 ! Enter post processor
PLNSOL,U,SUM,0,1 ! Plot deflection
WPOFFS,Width/2,0,0 ! Offset the working plane for cross-section view
WPROTA,0,0,90 ! Rotate working plane
/CPLANE,1 ! Cutting plane defined to use the WP
/TYPE,1,8 ! QSLICE display
WPCSYS,-1,0 ! Deflines working plane location
WPOFFS,0,0,1/16*Length ! Offset the working plane
/CPLANE,1 ! Cutting plane defined to use the WP
/TYPE,1,5 ! Use the capped hidden display
PLNSOL,S,EQV,0,1 ! Plot equivalent stress
!Animation
ANCUT,43,0.1,5,0.05,0,0.1,7,14,2 ! Animate the slices