Siemens SINUMERIK 840D Programming Manual page 170

Milling Cycles
3
3.12 Path milling - CYCLE72
Programming example 1
Milling a closed contour externally
This program is used to mill a contour as shown in
the figure.
Parameters for cycle call:
• Retraction plane
• Reference plane
• Safety clearance
• Depth
• Maximum depth infeed
• Final machining allowance
in depth
• Feedrate depth infeed
• Final machining allowance
in the plane
• Feedrate in the plane
• Machining: Roughing up to the finishing
Parameters for the approach:
• G41 - to the left of the contour, i.e. external
machining
• Approach and return on quadrant
in plane
• Retraction feedrate
%_N_RANDKONTUR1_MPF
;$PATH=/_N_MPF_DIR
N10 T20 D1
N15 M6
N20 S500 M3 F3000
N25 G17 G0 G90 X100 Y200 Z250 G94
N30 CYCLE72 ( "MYKONTUR", 250, 200, ->
-> 3, 175, 10,1, 1.5, 800, 400, 111, ->
-> 41, 2, 20, 1000, 2, 20)
N90 X100 Y200
N95 M02
-> Must be programmed in a single block
3-170
250 mm
200
3 mm
175 mm
10
1.5 mm
400 mm/min
1 mm
800 mm/min
allowance, intermediate travel with G1,
during the intermediate motions, return
along Z to _RFP + _SDIS
20 mm radius
1000 mm/min
Y
Contour starting point
Program for re-milling a contour with
CYCLE72
T20: milling cutter with radius 7
Changing tool T20
Program feedrate and spindle speed
Approach starting position
Cycle call
End of program
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
12.98
3
Programmed
contour direction
Final contour
Final contour + final
machining allowance
X
 Siemens AG 2000 All rights reserved.