!===============================================================================
! PROGRAM:          FE-Lab2 (Exercise 2)
! PROJECT:          FE Lab for Advanced Materials (U. Simon, www.uzwr.de)
! TASK:             Input file for Exercise 2:  Beam under 3-Point bending
!                   assuming symmetry (calculated as cantilever beam of half lenght)
! AUTHOR:           Simon U.
! LAST CHANGES:     2011 by Simon
!
! COMPUTER:         zeus.rz...
! OPERATING SYSTEM: Unix (SunOS)
! ANSYS Version:    License: aa_t_me, ANSYS v13
!
! CALL:             /input, FE-Lab2-v3.inp
!
!===============================================================================

!=== Init ======================================================================
FINISH              ! Stops all modules (preprocessor, solution, postprocessor)
/CLEAR              ! Start a new analysis, delete the old database (file.db)


!===============================================================================
!  Parameters (lenght in mm, forces in N => stiffnesses and stresses in N/mm)
!===============================================================================

! Use these parameters instead of numerical values so you can easily
! adapt your model (e.g. changed geometry, different load cases)

F_total       =   5000      ! force acting on full beam (N)
l_total       =   2000      ! length of the full beam (mm)
thickness     =     20      ! thickness of the beam (mm)
height        =     60      ! height of the beam (mm)
youngsMod     = 210000      ! Young's modulus of steel (MPa)
poissonsRatio =      0.3    ! Poisson's ratio of steel

!--- Dependent Parameters
F_half   = F_total/2         ! half force acting on cantilever beam
l_half   = l_total/2         ! half lenght of the cantilever beam

!===============================================================================
! A. Preprocessing - setting up the model
!===============================================================================
/PREP7                       ! Switch to the preprocessor module

!=== A.1 Build the geometry by means of bottom-up method
!--- A.1.1 Create keypoints
K, 1,    0.0, height/2, 0.0     ! Define keypoint 1 via its coordinates x1, y1, z1
K, 2, l_half, height/2, 0.0     ! Define keypoint via its coordinates x, y, z
!K, 3, ...
!K, 4, ...

!--- A 1.2 Create lines by connecting keypoints
!LSTR,                          ! Connect keypoints 1 and 2 to create line 1
!...
!...
!...

!--- A.1.3 Create area by connecting lines
!...                            ! 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 lines on
LPLOT                        ! Plot lines
!KPLOT                       ! Plot keypoints
!...                         ! Plot areas

!=== A.2 Material Properties
!--- A.2.1 Define material properties
!MP, ...                      ! Define Young's modulus for material No 1
!MP, ...                      ! Define Poisson's ratio for material No 1

!=== A.3 Meshing
!--- A.3.1 Define element type to be used for meshing
ET, 1, PLANE182              ! Define the local element type #1 to be PLANE182 element
KEYOPT, 1, 3, 3              ! Sets key option 3 (of elem type 1) to 3 (enables
                             ! "plane stress with thickn")

!--- A.3.2 Define real constants
R, 1, thickness              ! Sets thickness of the beam in "real set" no. 1

!--- A.3.3 Meshing
! select element type, material and real set used for meshing
TYPE, 1
MAT, 1
REAL, 1

! create mesh
!AMESH, 1                    ! Meshing area number 1
                             ! hint: you may also have a look at the commands
                             ! "mshkey" and "lesize" to control mesh refinement
!EPLOT                       ! Plot elements


!=== A.4 Apply Load and Boundary Conditions
!--- A.4.1 Displacement boundary conditions
!NSEL, S, LOC, X, 0.0        ! Select all nodes at x = 0 (left side)
!D, ALL, UX, 0.0             ! Set displacement ux to zero for all selected nodes
!D, ...                      ! Set displacement uy to zero for all 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)
! hint: NSEL- or *GET-command (read *GET documentation carefuly for a hidden
!       shortcut...)
!...
! apply force on this node:
!...

!===============================================================================
! B. Solution
!===============================================================================
!/SOLU                        ! Switch to the solution module


!=== B.1 Basic settings
!ANTYPE, 0                    ! Select the static analysis type

!--- B.2 start the calculation
!SOLVE                        ! Solve current load step


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


!=== C.1 Contour plots
!/DSCALE, 1, 1.0              ! Switch off auto scaling of deformed shape
! plot displacement, stresses, etc.
!...