HEIDENHAIN TNC 640 User Manual page 414

12
Q487 Allow plunging (0/1)?: Permit machining of
plunging elements:
0: Do not machine plunging elements
1: Machine plunging elements
Q488 Feed rate for plunging (0=auto)?: Feed rate
for machining plunging elements. This input value
is optional. If it is not programmed, then the feed
rate defined for turning operations applies.
Q479 Machining limits (0/1)? : Activate cutting
limit:
0: No cutting limit active
1: Cutting limit (Q480/Q482)
Q480 Value of diameter limit?: X value for
contour limitation (diameter value)
Q482 Value of cutting limit in Z?: Z value for
contour limitation
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°
414
Cycles: Turning | TURN CONTOUR FACE
(Cycle 820, DIN/ISO: G820)
Q478=+0.3 ;ROUGHING FEED RATE
Q483=+0.4 ;OVERSIZE FOR DIAMETER
Q484=+0.2 ;OVERSIZE IN Z
Q505=+0.2 ;FINISHING FEED RATE
Q487=+1 ;PLUNGE
Q488=+0 ;PLUNGING FEED RATE
Q479=+0 ;CONTOUR MACHINING
LIMIT
Q480=+0 ;DIAMETER LIMIT VALUE
Q482=+0 ;LIMIT VALUE Z
Q506=+0 ;CONTOUR SMOOTHING
12 L X+75 Y+0 Z+2 FMAX M303
13 CYCL CALL
14 M30
15 LBL 2
16 L X+75 Z-20
17 L X+50
18 RND R2
19 L X+20 Z-25
20 RND R2
21 L Z+0
22 LBL 0
HEIDENHAIN | User's manual for cycle programming | 10/2017