Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | TURN CONTOUR FACE
(Cycle 820, DIN/ISO: G820)

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? (incremental): Distance
for retraction and pre-positioning.
Q499 Reverse the contour (0-2)?: Define the
machining direction of the contour:
0: Contour machined in the programmed direction
1: Contour machined in reverse direction to the
programmed direction
2: Contour machined in reverse direction to the
programmed direction; additionally, the orientation
of the tool is adjusted
Q463 Maximum cutting depth?: Maximum infeed
in axial direction. The infeed is divided evenly to
avoid abrasive cuts.
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.
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q460
Q484
NC blocks
9 CYCL DEF 14.0 CONTOUR
10 CYCL DEF 14.1 CONTOUR LABEL2
11 CYCL DEF 820 TURN CONTOUR
TRANSV.
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q499=+0 ;REVERSE CONTOUR
Q463=+3 ;MAX. CUTTING DEPTH
12
Q463
Ø Q483
413