HEIDENHAIN TNC 620 User Manual page 111

Fixed Cycles: Drilling | Programming Examples
8 L Z+100 R0 FMAX
9 TOOL CALL 2 Z S5000
10 L Z+50 R0 F5000
11 CYCL DEF 200 DRILLING
Q200=2 ;SET-UP CLEARANCE
Q201=-25 ;DEPTH
Q206=150 ;FEED RATE FOR PLNGNG
Q202=5 ;PLUNGING DEPTH
Q211=0 ;DWELL TIME AT TOP
Q203=+0 ;SURFACE COORDINATE
Q204=10 ;2ND SET-UP CLEARANCE
Q211=0.2 ;DWELL TIME AT DEPTH
Q395=0 ;DEPTH REFERENCE
12 CYCL CALL PAT F500 M13
13 L Z+100 R0 FMAX
14 TOOL CALL Z S200
15 L Z+50 R0 FMAX
16 CYCL DEF 206 TAPPING NEW
Q200=2 ;SET-UP CLEARANCE
Q201=-25 ;DEPTH OF THREAD
Q206=150 ;FEED RATE FOR PLNGNG
Q211=0 ;DWELL TIME AT DEPTH
Q203=+0 ;SURFACE COORDINATE
Q204=10 ;2ND SET-UP CLEARANCE
17 CYCLE CALL PAT F5000 M13
18 L Z+100 R0 FMAX M2
19 END PGM 1 MM
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
Retract the tool, change the tool
Call the drilling tool (radius 2.4)
Move tool to clearance height
Cycle definition: drilling
Call the cycle in connection with the hole pattern
Retract the tool
Call the tapping tool (radius 3)
Move tool to clearance height
Cycle definition for tapping
Call the cycle in connection with the hole pattern
Retract the tool, end program
3
111