Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | TURN SHOULDER FACE
(Cycle 821, DIN/ISO: G821)

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.
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
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.
Q506 Contour smoothing (0/1/2)?:
0: After each cut along the contour (within the
infeed range)
1: Contour smoothing after the last cut (complete
contour); retract below 45°
2: No contour smoothing; retract below 45°
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q460
Q484
NC blocks
11 CYCL DEF 821 SHOULDER, FACE
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q493=+30 ;DIAMETER AT CONTOUR
END
Q494=-5 ;CONTOUR END IN Z
Q463=+3 ;MAX. CUTTING DEPTH
Q478=+0.3 ;ROUGHING FEED RATE
Q483=+0.4 ;OVERSIZE FOR DIAMETER
Q484=+0.2 ;OVERSIZE IN Z
Q505=+0.2 ;FINISHING FEED RATE
Q506=+0 ;CONTOUR SMOOTHING
12 L X+75 Y+0 Z+2 FMAX M303
13 CYCL CALL
12
Q463
Ø Q493
Ø Q483
399