Cycle Parameters - HEIDENHAIN TNC 640 User Manual

12

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
Q493 Diameter at end of contour?: X coordinate
of the contour end point (diameter value)
Q493 Contour end in Z?: Z coordinate of the
contour end point
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.
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
452
Cycles: Turning | AXIAL RECESSING
(Cycle 871, DIN/ISO: G871)
Q494
Q484
NC blocks
11 CYCL DEF 871 SIMPLE RECESS, AXIAL
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q493=+50 ;DIAMETER AT CONTOUR
END
Q494=-10 ;CONTOUR END IN Z
Q478=+0.3 ;ROUGHING FEED RATE
Q483=+0.4 ;OVERSIZE FOR DIAMETER
Q484=+0.2 ;OVERSIZE IN Z
Q505=+0.2 ;FINISHING FEED RATE
Q463=+0 ;LIMIT TO DEPTH
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q460
Q463
Ø Q493
Ø Q483