HEIDENHAIN TNC 620 User Manual page 406

11
Programming: Special Functions
11.4 Working with the parallel axes U, V and W
Example: Drilling in the W axis
0 BEGIN PGM PAR MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 5 Z S2222
4 L Z+0 W+0 R0 FMAX M91
5 L Z+100 R0 FMAX M3
6 CYCL DEF 200 DRILLING
Q200=+2
Q201=-20
Q206=+150
Q202=+5
Q210=+0
Q203=+0
Q204=+50
Q211=+0
Q395=+0
7 FUNCTION PARAXCOMP DISPLAY Z W
8 FUNCTION PARAXMODE X Y W
9 L X+50 Y+50 R0 FMAX M99
10 FUNCTION PARAXMODE OFF
11 L Z+0 W+0 R0 FMAX M91
12 L M30
13 END PGM PAR MM
406
;SET-UP CLEARANCE
;DEPTH
;FEED RATE FOR PLNGNG
;PLUNGING DEPTH
;DWELL TIME AT TOP
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;DWELL TIME AT DEPTH
;DEPTH REFERENCE
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2015
Call the tool in the spindle axis Z
Reset the principle axis and minor axis
Position the principal axis
Activate display compensation
Positive axis selection
Infeed runs minor axis W
Restore standard axis configuration
Reset the principle axis and minor axis