Second Programming Example For Milling Application - Siemens SINUMERIK 840Di sl Programming Manual

Example
_MILL1_MPF
N10 MSG("THIS IS MY NC PROGRAM")
:10 F200 S900 T1 D2 M3
N20 G0 X100 Y100
N30 G1 X150
N40 Y120
N50 X100
N60 Y100
N70 G0 X0 Y0
N100 M30
2.5

Second programming example for milling application

Programming a sample workpiece
This programming example contains surface and side milling, as well as drilling.
• The workpiece is intended for machining on a vertical milling machine.
• The dimensions are in inches.
Machine manufacturer
The machine data settings must be defined correctly before the program can run on the
machine.
References: /FB1/Function Manual Basic Functions; Axes, Coordinate Systems,.. (K2)
Example
%_N_RAISED_BOSS_MPF
N005 MSG ("Traverse axes to tool change location")
N010 START01:SUPA G0 G70 Z0 D0
N015 SUPA X0 Y0
;********************Tool change********************
N020 MSG ("Tool change active")
N025 T1 M6
N030 MSG ()
N035 MSG ("Face milling Z=0 workpiece surface")
N040 G0 G54 X-2 Y.6 S800 M3 M8
N045 Z1 D1
N050 G1 Z0 F50
N055 X8 F25
N060 G0 Y3.5
N065 G1 X-2
Fundamentals
Programming Manual, 11/2006, 6FC5398-1BP10-2BA0
Fundamental Principles of NC Programming
2.5 Second programming example for milling application
;MSG = Message output in an alarm line
;Feed, spindle, tool,
;tool offset, spindle clockwise
;Rapid traverse to position
;Rectangle with feed, straight line in X
;Straight line in Y
;Straight line in X
;Straight line in Y
;Return rapid traverse movement
;End of block
;d = 3 inch face cutter
;Clears the message from block N020
71