Siemens SINUMERIK 840D Programming Manual page 161

03.96
3
05.98
Programming example
Face milling
Parameters for cycle call:
• Retraction plane:
• Reference plane:
• Safety clearance:
• Milling depth:
• Max. infeed depth
• No final machining allowance
• Starting point of the rectangle
• Rectangle dimensions
• Angle of rotation in the plane
• Max. infeed width
• Retraction travel at the end of
the milling path:
• Feedrate for surface machining
• Type of machining: roughing parallel to the X axis
with changing direction
• Overrun on last cut as determined by the cutting
edge geometry
%_N_TSTCYC71_MPF
;$PATH=/_N_MPF_DIR
;*
$TC_DP1[1,1]=120
$TC_DP6[1,1]=10
N100 T1
N102 M06
N110 G17 G0 G90 G54 G94 F2000 X0 Y0
Z20
;
CYCLE71( 10,
-> 60, 40, 10, 6, 10, 5, 0, 4000, 31, 2)
N125 G0 G90 X0 Y0
N130 M30
-> Must be programmed in a single block
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
10 mm
0 mm
2 mm
-11 mm
6 mm
X = 100 mm
Y = 100 mm
X = +60 mm
Y = +40 mm
10 degrees
10 mm
5 mm
4000 mm/min
2 mm
0, 2,-11, 100, 100, ->
3.11 Face milling - CYCLE71
Program for face milling with CYCLE71
Tool type
Tool radius
Approach starting position
Cycle call
End of program
Milling Cycles
3
3-161