Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | AXIAL RECESSING
(Cycle 870, DIN/ISO: G870)

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.
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
Q463 Limit to plunging depth?: Max. recess
depth per cut
Q510 Overlap factor for recess width? The
factor Q510 influences the stepover of the tool
when roughing. Q510 is multiplied by the width
CUTWIDTH of the tool. This results in the stepover
factor "k". Input range 0.001 to 1
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 870 CONT. RECESS, AXIAL
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q478=+0.3 ;ROUGHING FEED RATE
Q483=+0.4 ;OVERSIZE FOR DIAMETER
Q484=+0.2 ;OVERSIZE IN Z
Q505=+0.2 ;FINISHING FEED RATE
Q479=+0 ;CONTOUR MACHINING
LIMIT
Q480=+0 ;DIAMETER LIMIT VALUE
Q482=+0 ;LIMIT VALUE Z
12
Q460
Ø Q483
Q463
461