##

The first step is to simplify the problem. Whenever you are trying out a new analysis type, you need something (ie analytical solution or experimental data) to compare the results to. This way you can be sure that you've gotten the correct analysis type, units, scale factors, etc.

The simplified version that will be used for this problem is that of a flat rectangular plate with a hole shown in the following figure:

## ANSYS Command Listing

! Command File mode of 2D Plane Stress Verification
/title, 2D Plane Stress Verification
/PREP7 ! Preprocessor
BLC4,0,0,200,100 ! rectangle, bottom left corner coords, width, height
CYL4,100,50,20 ! circle,center coords, radius
ASBA,1,2 ! substract area 2 from area 1
ET,1,PLANE42 !element Type = plane 42
KEYOPT,1,3,3 ! This is the changed option to give the plate a thickness
R,1,20 ! Real Constant, Material 1, Plate Thickness
MP,EX,1,200000 ! Material Properties, Young's Modulus, Material 1, 200000 MPa
MP,PRXY,1,0.3 ! Material Properties, Major Poisson's Ratio, Material 1, 0.3
AESIZE,ALL,5 ! Element sizes, all of the lines, 5 mm
AMESH,ALL ! Mesh the lines
FINISH ! Exit preprocessor
/SOLU ! Solution
ANTYPE,0 ! The type of analysis (static)
DL,4, ,ALL,0 ! Apply a Displacement to Line 4 to all DOF
SFL,2,PRES,-1 ! Apply a Distributed load to Line 2
SOLVE ! Solve the problem
FINISH
/POST1
PLNSOL,S,EQV