Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | AXIAL RECESSING
(Cycle 850, DIN/ISO: G850)

Cycle parameters

Q215 Machining operation (0/1/2/3)?: Define
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing to finished dimension
3: Only finishing to oversize
Q460 Set-up clearance?: Reserved, currently
without function
Q478 Roughing feed rate?: Feed rate for
roughing. If M136 has been programmed, the
value is interpreted by the TNC in millimeters
per revolution, without M136 in millimeters per
minute.
Q488 Feed rate for plunging (0=auto)?: Feed rate
for machining plunging elements. This input value
is optional. If it is not programmed, then the feed
rate defined for turning operations applies.
Q483 Oversize for diameter? (incremental):
Diameter oversize for the defined contour
Q484 Oversize in Z? (incremental): Oversize for
the defined contour in axial direction
Q505 Finishing feed rate?: Feed rate for
finishing. If M136 has been programmed, the
value is interpreted by the TNC in millimeters
per revolution, without M136 in millimeters per
minute.
Q479 Machining limits (0/1)? : Activate cutting
limit:
0: No cutting limit active
1: Cutting limit (Q480/Q482)
Q480 Value of diameter limit?: X value for
contour limitation (diameter value)
Q482 Value of cutting limit in Z?: Z value for
contour limitation
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q484
NC blocks
9 CYCL DEF 14.0 CONTOUR
10 CYCL DEF 14.1 CONTOUR LABEL2
11 CYCL DEF 850 RECESS TURNG, AXIAL
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q478=+0.3 ;ROUGHING FEED RATE
Q488=0 ;PLUNGING FEED RATE
Q483=+0.4 ;OVERSIZE FOR DIAMETER
Q484=+0.2 ;OVERSIZE IN Z
Q505=+0.2 ;FINISHING FEED RATE
12
Q460
Q463
Ø Q483
435