HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 313)

TURN SHOULDER FACE
(Cycle 821, DIN/ISO: G821)
13.11
13
TNC 640 | User's Manual Cycle Programming | 5/2013
313
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 (incremental): Distance for
retraction and pre-positioning
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
Maximum cutting depth Q463: Maximum infeed in
axial direction. The infeed is divided evenly to avoid
abrasive cuts.
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.
Contour smoothing Q506:
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°
Q460
Ø Q493
Q463
Ø Q483
Q484
NC blocks
11 CYCL DEF 821 TURN SHOULDER
FACE
Q215=+0 ;MACHINING OPERATION
Q460=+2 ;SAFETY CLEARANCE
Q493=+30 ;DIAMETER AT END OF
CONTOUR
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