Contour Milling - Cycle72 - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

Parameter
_WID
_STA
_MID
_MIDA
_FDP
_FALD
_FFP1
_VARI
_FDP1
A milling cutter with 10 mm radius is used.
N10 T2 D2
N20 G17 G0 G90 G54 G94 F2000 X0 Y0 Z20
N30 CYCLE71(10, 0, 2, -11, 100, 100, 60, 40, 10, 6, 10, 5,
0, 4000, 31, 2)
N40 G0 G90 X0 Y0
N50 M02
9.6.3

Contour milling - CYCLE72

Programming
CYCLE72 (_KNAME, _RTP, _RFP, _SDIS, _DP, _MID, _FAL, _FALD, _FFP1, _FFD, _VARI, _RL, _AS1, _LP1, _FF3, _AS2,
_LP2)
Parameters
Parameter Data type
_KNAME STRING
_RTP REAL
_RFP REAL
_SDIS REAL
_DP REAL
_MID REAL
_FAL REAL
_FALD REAL
_FFP1 REAL
_FFD REAL
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
Description
Rectangle dimensions
Angle of rotation in the plane
Maximum infeed depth
Maximum infeed width
Retraction at the end of the milling path
Finishing allowance in depth
Feedrate in the plane
Machining type
Overrun on last cut as determined by the cutting
edge geometry
Description
Name of contour subroutine
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (to be added to the reference plane; enter without sign)
Depth (absolute)
Maximum infeed depth (incremental; enter without sign)
Finishing allowance at the edge contour (enter without sign)
Finishing allowance at the base (incremental, enter without sign)
Feedrate for surface machining
Feedrate for depth infeed (enter without sign)
Value
Y = +40 mm
10 degrees
6 mm
10 mm
5 mm
No finishing allowance
4000 mm/min
31 (Roughing parallel to the X axis with
alternating direction)
2 mm
; Approach start position
; Cycle call
; End of program
167