Long Holes Located On A Circle - Longhole - Siemens SINUMERIK 808D User Manual

N o te
A tool compensation must be programmed before the cycle is called. Otherwise, the cycle is canceled and alarm 61009
"Active tool number=0" is output. Internally in the cycle, a new current workpiece coordinate system is used which influences
the actual value display. The zero point of this coordinate system is to be found in the pocket center point.
At the end of the cycle, the original coordinate system is active again.
Programming example: Circular spigot
Machining a spigot from a blank with a diameter of 55 mm and a maximum infeed of 10 mm per cut; specification of a final
machining allowance for subsequent finishing of the spigot surface. The whole machining is performed with reverse rotation.
See the following programming example for circular spigot:
N10 G90 G17 G0 S1800 M3 D1 T1
N11 M6
N20 CYCLE77 (10, 0, 3, -20, ,50, 60, 70, 10, 0.5, 0, 900,
800, 1, 1, 55)
N30 D1 T2 M6
N40 S2400 M3
N50 CYCLE77 (10, 0, 3, -20, , 50, 60, 70, 10, 0, 0, 800,
800, 1, 2, 55)
N40 M30
12.6.6

Long holes located on a circle - LONGHOLE

Programming
LONGHOLE (RTP, RFP, SDIS, DP, DPR, NUM, LENG, CPA, CPO, RAD, STA1, INDA, FFD, FFP1, MID)
Pa rameters
Pa rameter D a ta type
RTP REAL
RFP REAL
SDIS REAL
DP REAL
DPR REAL
NUM INT
LENG REAL
CPA REAL
CPO REAL
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
D e scription
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (enter without sign)
Slot depth (absolute)
Slot depth relative to the reference plane (enter without sign)
Number of slots
Slot length (enter without sign)
Center point of circle (absolute), first axis of the plane
Center point of circle (absolute), second axis of the plane
; Specification of technology values
; Roughing cycle call
; Change tool
; Specification of technology values
; Call finishing cycle
; End of program
207