HEIDENHAIN TNC 620 User Manual page 64

2
Example
0 BEGIN PGM C200 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 5 Z S4500
4 L Z+250 R0 FMAX M3
5 PATTERN DEF
POS1 (X+10 Y+10 Z+0)
POS2 (X+10 Y+90 Z+0)
POS3 (X+90 Y+90 Z+0)
POS4 (X+90 Y+10 Z+0)
6 CYCL DEF 200 DRILLING
Q200=2
Q201=-20
Q206=250
Q202=5
Q210=0
Q203=-10
Q204=20
Q211=0.2
Q395=0
7 CYCL CALL PAT FMAX M8
8 L Z+250 R0 FMAX M30
9 END PGM C200 MM
Further information on this topic
Creating a new NC program
Further information: "Creating and entering NC programs",
Page 90
Cycle programming
Further information: User's Manual for Programming of
Machining Cycles
64
;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
First steps | Programming the first part
Workpiece blank definition
Tool call
Retract the tool; turn on spindle
Define the machining positions
Define the cycle
Turn on coolant; call cycle
Retract the tool, end program
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022