!===============================================================================
! ANSYS CLASSIC 
!===============================================================================
! PROJEKT:          MOSI 2 (B. Wieland, U. Simon, K.Becker-Steinberger
!                   www.uni-ulm.de/uzwr)
!                   UEBUNG 02 "3-Punkt Biegung, APDL Skripts in ANSYS Classical"
! PROGRAM:          blatt2.inp
! DATE:             04.05.2012
! AUTHORS:          B. Wieland, U. Simon, K.Becker-Steinberger
! 
! COMPUTER:         zeus.rz.uni-ulm.de
! ANSYS Version:    License: Academic Teaching Advanced, Version: 13.0
! 
! CALL:             /input,blatt2.inp
!===============================================================================


!===============================================================================
! BEGINNING
!===============================================================================
FINISH              ! Stops all modules (preprocessor, solution, postprocessor)
/CLEAR              ! Clears an existing database to start a new analysis


!===============================================================================
! PARAMETER AND CONSTANTS 
!    lengths      in mm
!    forces       in N
!    stiffnesses  in N/mm = MPa
!    stresses     in N/mm = MPa
!===============================================================================
length =   1000.0                ! length of the full beam
height =     60.0                ! height of the beam
width  =     20.0                ! thickness of the beam
force  =   2500.0                ! force acting on full beam

e_modul     = 210000.0           ! Young's Modulus of the beam's material (steel)
poissonzahl =      0.3           ! Poisson's Ratio of the beam's material (steel)

nofel_horizontal = 24            ! Number of Elements in horizontal direction
nofel_vertical  = 4              ! Number of Elements in horizontal direction

!===============================================================================
!===== A. PREPROCESSOR =========================================================
!===============================================================================
/PREP7                           ! Switch to the preprocessor module


!===============================================================================
! A.1 BUILD THE GEOMETRY 
!===============================================================================

!===== A.1.1 CRETAE KEYPOINTS ==================================================
K, 1,    0.0,  height/2, 0.0     ! Define keypoint 1 via its coordinates x, y, z
K, 2, length,  height/2, 0.0     ! Define keypoint 2 via its coordinates x, y, z
K, 3, length, -height/2, 0.0     ! Define keypoint 3 via its coordinates x, y, z
K, 4,    0.0, -height/2, 0.0     ! Define keypoint 4 via its coordinates x, y, z

!===== A.1.2 CREATE LINES BY CONNECTING KEYPOINTS ==============================
LSTR, 1, 2                       ! Connect keypoints 1 and 2 to create line 1
LSTR, 2, 3                       ! Connect keypoints to create a line
LSTR, 3, 4                       ! Connect keypoints to create a line
LSTR, 4, 1                       ! Connect keypoints to create a line

!===== A.1.3 CREATE AREA VIA CONNECTING THE LINES ==============================
AL, 1, 2, 3, 4                   ! Create area 1 by lines 1, 2, 3, 4

!===== A.1.4 VISUALIZATION OF THE CREATED ELEMENTS =============================
/PNUM, KP, 1                     ! Switch numbering of keypoints on
/PNUM, LINE, 1                   ! Switch numbering of lines on
/PNUM, AREA, 1                   ! Switch numbering of areas on
KPLOT                            ! Plot keypoints
LPLOT                            ! Plot lines
APLOT                            ! Plot areas


!===============================================================================
! A.2 MESHING 
!===============================================================================

!===== A.2.1 ASSIGN THE ELEMENT TYPE ===========================================
ET, 1, plane182                  ! Define local element type 1 as PLANE182 element
KEYOPT, 1, 3, 3                  ! Sets for element type 1 the key option 3 to 3
                                 ! (plane stress with thickness)
!===== A.2.2 MESHING ===========================================================
!--- Simple mesh size controll
! SMRTSIZE,4                     ! Smart sizing, 1=fine to 10=coarse

!- Better mesh size controll
MSHKEY, 1                        ! Mapped meshing (1) or free meshing (0)
LESIZE, 1,,,nofel_horizontal     ! Horizontal: Element devisions on line 1
LESIZE, 4,,,nofel_vertical       ! Vertical:   Element devisions on line 4
AMESH, 1                         ! Mesh area number 1
EPLOT                            ! Plot elements


!===============================================================================
! A.3 MATERIAL PROPERTIES
!===============================================================================

!===== A.3.1 DEFINE REAL CONSTANTS =============================================
R, 1, width                      ! Set thicknessess of the beam in "real set" no. 1

!===== A.3.2 DEFINE MATERIAL PROPERTIES ========================================
MP, EX, 1, e_modul               ! Define Young's modulus for material no. 1
MP, PRXY, 1, poissonzahl         ! Define Poisson's Ratio for material no. 1



!===============================================================================
! A.4 APPLY LOAD AND BOUNDARY CONDITIONS
!===============================================================================

!===== A.4.1 DISPLACEMENT BOUNDARY CONDITION ===================================
NSEL, S, LOC, X, 0.0             ! Select all nodes at x = 0 (left side)
D, ALL, UX, 0.0                  ! Set displacement ux to 0 for selected nodes

D, NODE(0.0, 0.0, 0.0), UY, 0.0  ! Set displacement uy to 0 for selected nodes
ALLSEL                           ! Re-select all entities 

!===== A.4.2 APPLYING THE LOADS ================================================
!- Get node number of node at location x, y, z (lower right corner)
nodenum = NODE(length, 0.0, 0.0)
F, nodenum, FY, force            ! Apply load on node "nodenum"




!===============================================================================
!===== B. Solution =============================================================
!===============================================================================
/SOLU                            ! Switch to the solution module
ANTYPE, 0                        ! Select the static analysis type 
SOLVE                            ! Solve current load step


!===============================================================================
!===== C. Postprocessor ========================================================
!===============================================================================
/POST1                           ! Switch to the postprocessor module

!===== C.0.1 CONTOUR PLOT DISPLACEMENT =========================================
/DSCALE, 1, 1.0                  ! Switch off auto scaling of deformed shape
/TITLE,Displacement: u_y in mm   ! Define a caption on the plot
PLNSOL, U, Y, 2                  ! Contour plot of vertical displacements

!===== C.0.2 CONTOUR PL0T NORMAL STRESS IN X-DIRECTION =========================
/TITLE,Normal stress in x-direction: sigma_xx in MPa
PLESOL, S, X, 2                  ! Plot the deformed shape with normal stress in x