/TITLE, Your name and date here, thermex04.a 
     ! element 1, 2 steel, elements 3 aluminum
	 ! fixed on left end, 25F temperature change
/PREP7
p2 = -2*4e3     ! Load at node 2
p3 = -2*2e3     ! Load at node 3
p4 = 10e3       ! Load at node 3
temper = 25     ! temperature
dia1 = 1.5
dia2 = 1.2
pi = 4*atan(1)

ET,1,Pipe16        ! Type 16 is a pipe
R,1,dia1,(dia1/2)  ! OD, wall
R,2,dia2,(dia2/2)
MP,EX,1,29e6       ! Young-s modulus, steel
MP,EX,2,11e6       ! Young-s modulus, aluminum
MP,ALPX,1,6.5e-6   ! thermal expansion, steel
MP,ALPX,2,13.1e-6  ! thermal expansion, aluminum

N,1,0              ! Node 1 at 0
N,2,(2*12)         ! Node 2
N,3,((2+3)*12)     ! Node 3
N,4,((2+3+4)*12)   ! Node 4

TYPE,1             ! element type1 (spar)
REAL,1             ! area R 1
MAT,1              ! material property MP 1 (steel)
E,1,2              ! Element 1, nodes 1-2
E,2,3              ! Element 2
REAL,2             ! Area 2
MAT,2              ! material property MP 2 (aluminum)
E,3,4              ! Element 3
FINISH

/solution
antype,static
outpr,basic,1
outpr,nload,1
D,1,ALL,0        ! Fix node 4
F,2,FX,p2        ! Force at node 2
F,3,FX,p3        ! Force at node 3
F,4,FX,p4        ! Force at node 1
BFE,ALL,TEMP,1,temper  ! Temperature all elements
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

!     NODE      UX       
!        1   0.0000      
!        2  0.29634E-02  
!        3  0.13028E-01  
!        4  0.67331E-01  

!     NODE      FX       
!        1   2000.0       
 
!     ELEM    STR     
!        1  -1131.8    
!        2   3395.3    
!        3   8841.9