!It is good practice to give a meaningful title such as:
!Cantilever beam problem from a previous assignment (HW4, Prob2)
!The following are ANSYS commands to cut and paste into ANSYS.

!UNITS: all units will be based on pounds (force) and inches

FINI	!Good practice to make sure to begin fresh –FINI (finish) tells ANSYS to finish any previous work
/CLEAR	!Clears any previous activity
/BATCH	!Works in “batch” mode
/PREP7	!Enter the preprocessor

!Define Beam Geometry parameters.  We do not need to define the following, we can directly enter values into the commands, but structuring the code this way allows for easy changes later.

HEIGHT=2
WIDTH=0.25
LENGTH=40
ELEMLENGTH=40    !total number of elements will be LENGTH/ELEMLENGTH – or the nearest integer.

!Define locations of key points.  Key points will be discussed later. For now, understand that key points can be helpful in creating geometry.
K,1,0,0,0
K,2,LENGTH,0,0    ! We have already defined LENGTH=40; this line could be typed as K,2,40,0,0
L,1,2	!Create a line connecting Key Points 1 and 2.

!Define element information:
ET,1,BEAM189	!BEAM189 is a beam element (line element)
SECTYPE,1,BEAM,RECT	!Defines the cross-section of the beam as a rectangle.  Many common structural shapes can be easily defined with the command SECTYPE including I-Beams.
SECOFFSET,CENT	!This sets the beam node to be located at the beam’s cross-sectional centroid.
SECDATA,HEIGHT,WIDTH   !we have defined HEIGHT and WIDTH
MP,EX,1,29e6	!MP = Material Property, EX is Modulus of elasticity
!NOTE: units for Young’s modulus MUST be the same unit of force and length as used elsewhere
MP,PRXY,1,0.3  !PRXY is Poisson’s ratio
ESIZE, ELEMLENGTH   !Define element size as ELEMLENGTH defined above
LMESH,ALL	!Mesh the line – in other words, create the elements
FINI		!Finish the preprocessing

/SOLU		!Enter the solution processor (define loads and constraints)
DK,1,ALL,0	!you will be asked to look up this command in ANSYS Help.
FK,2,FY,-1000	!you will be asked to look up this command in ANSYS Help.
ALLSEL		!you will be asked to look up this command in ANSYS Help.
SOLVE		!Solve the model
FINI		!Finish and exit “solution”

/POST1		!Enter the general post-processor
/ESHAPE,1	!Display element shapes using section data
/DSCALE,ALL,1	!Plot using true scale
/VIEW,1,1,1,1	!Isometric view
FINI		!Finish and exit the post-processor
SAVE		!Save the data base