Siemens SINUMERIK 808D User Manual page 191

● Tens digit:
1=parallel to the first axis of the plane; unidirectional
2=parallel to the second axis of the plane; unidirectional
3=parallel to the first axis of the plane; with alternating direction
4=parallel to the second axis of the plane; with alternating direction
If a different value is programmed for the parameter _VARI, the cycle is aborted after output of alarm 61002 "Machining type
defined incorrectly".
N o te
A tool compensation must be programmed before the cycle is called. Otherwise, the cycle is aborted and alarm 61000 "No
tool compensation active" is output.
Programming example: Face milling
Parameters for the cycle call:
Pa rameter
_RTP
_RFP
_SDIS
_DP
_PA
_PO
_LENG
_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
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
D e scription
Retraction plane
Reference plane
Safety clearance
Milling depth
Starting point of the rectangle
Starting point of the rectangle
Rectangle dimensions
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
Va lue
10 mm
0 mm
2 mm
-11 mm
X = 100 mm
Y = 100 mm
X = +60 mm
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
191