Please Note While Programming; Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Contour Pocket | FLOOR FINISHING (Cycle 23, DIN/ISO: G123)

Please note while programming:

The TNC automatically calculates the starting point for
finishing. The starting point depends on the available
space in the pocket.
The approaching radius for pre-positioning to the final
depth is permanently defined and independent of the
plunging angle of the tool.
If M110 is activated during operation, the feed rate
of compensated circular arcs within will be reduced
accordingly.
Danger of collision!
If you set the parameter posAfterContPocket to
ToolAxClearanceHeight, the TNC positions the tool after the end
of the cycle only in the tool axis direction to the clearance height.
The TNC does not position the tool in the working plane.
After the end of the cycle, position the tool with all
coordinates of the working plane, e.g.
After the cycle, program the absolute position (not an
incremental traversing movement)

Cycle parameters

Q11 Feed rate for plunging?: Traversing speed of
the tool in mm/min while plunging. Input range 0
to 99999.9999, alternatively FAUTO, fu, FZ
Q12 Feed rate for roughing?: Traversing speed
of the tool in the working plane. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q208 Feed rate for retraction?: Traversing speed
of the tool in mm/min when retracting after the
machining operation. If you enter Q208 = 0, the
TNC retracts the tool at the feed rate Q12. Input
range 0 to 99999.9999, alternatively fmax,FAUTO
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
L X+80 Y+0 R0 FMAX
NC blocks
60 CYCL DEF 23 FLOOR FINISHING
Q11=100 ;FEED RATE FOR PLNGNG
Q12=350 ;FEED RATE F. ROUGHNG
Q208=9999 ;RETRACTION FEED RATE
7
233