/TITLE, Your name, ME 421, and date here, axial1.a
  ! Ansys program for displacement and stress
  ! of axial forces on stepped bar, right end fixed

/PREP7           ! preprocessor section
p1 = 1000        ! Load at node 1
dia1 = 1.1
dia2 = 1.6

ET,1,Pipe16      ! type 16 is a pipe
R,1,dia1,dia1/2  ! diam, wall thickness
R,2,dia2,dia2/2

!  the following is an alternative method
! pi = (4*atan(1))
! ET,1,Link1         ! Type 1 is a spar or link
! R,1,(pi/4*dia1**2) ! Area 1
! R,2,(pi/4*dia2**2) ! Area 2

MP,EX,1,29e6     ! Young's modulus, steel
MP,EX,2,11e6     ! Young's modulus, aluminum

N,1,0            ! node 1 at 0
N,2,10           ! node 2 at 10
N,3,(10+12)      ! node 3 at 22

TYPE,1           ! element type1 (pipe)
REAL,1           ! area R 1
MAT,1            ! material property MP 1 (steel)
E,1,2            ! element 1, nodes 1-2
REAL,2           ! area R 2
MAT,2            ! material property MP 2 (aluminum)
E,2,3            ! element 2, nodes 2-3
FINISH           ! preprocessor section

/SOLUTION        ! solution section
antype,static    ! analysis type is static
outpr,basic,1
outpr,nload,1
D,3,ALL,0        ! node 3 fully constrained
F,1,FX,p1        ! force at node 1
solve
/PBC,ALL,1
FINISH           ! solution section

/POST1           ! post processor
etable,STR,ls,1,3
pldisp,1           ! plot displacements
! /output,Displ,txt,D:\Ansys\   !  displacements
 /output,Displ,txt,U:\win\Ansys\   !  displacements

PRNSOL,U           ! show displacements
! /output,Stress,txt,D:\Ansys\   !  forces and stresses
 /output,Stress,txt,U:\win\Ansys\   !  forces and stresses
PRRSOL             ! show forces
PRETAB             ! stresses
! FINISH           ! post processor

! End of Ansys program

! The following is the output from this program

!    NODE      UX
!      1    0.90542E-03
!      2    0.54257E-03
!      3    0.

!    NODE      FX
!      3    -1000.00

!   ELEM    STR
!      1  -1052.3
!      2   -497.36