/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