HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 364)

Cycles: Turning
13.25 AXIAL RECESSING
(Cycle 871, DIN/ISO: G871)
13
364
TNC 640 | User's Manual Cycle Programming | 5/2013
Please note while programming:
Program a positioning block to the starting position
with radius compensation
R0 before the cycle call.
The tool position at cycle call defines the size of the
area to be machined (cycle starting point).
Cycle parameters
Machining operation Q215: Define machining
operation:
0 : Roughing and finishing
1 : Only roughing
2 : Only finishing to finished dimension
3 : Only finishing to oversize
Set-up clearance Q460: Reserved, currently
without function
Diameter at end of contour Q493: X coordinate of
the contour end point (diameter value)
Contour end in Z Q494: Z coordinate of the contour
end point
Roughing feed rate Q478: Feed rate during
roughing. If M136 has been programmed, the
value is interpreted by the TNC in millimeters per
revolution, without M136 in millimeters per minute.
Oversize in diameter Q483 (incremental): Diameter
oversize for the defined contour
Oversize in Z Q484 (incremental): Oversize for the
defined contour in axial direction
Finishing feed rate Q505: Feed rate during
finishing. If M136 has been programmed, the
value is interpreted by the TNC in millimeters per
revolution, without M136 in millimeters per minute.
Limit to depth Q463: Max. recess depth per cut
Q460
Ø Q493
Q494
Q463
Ø Q483
Q484
NC blocks
11 CYCL DEF 871 AXIAL RECESSING
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q493=+50 ;DIAMETER AT END OF
CONTOUR
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
12 L X+65 Y+0 Z+2 FMAX M303
13 CYCL CALL