HEIDENHAIN ITNC 530 - CYCLE PROGRAMMING User Manual page 104

6 CYCL DEF 240 CENTERING
Q200=2 ;SETUP CLEARANCE
Q343=0 ;SELECT DEPTH/DIA.
Q201=-2 ;DEPTH
Q344=-10 ;DIAMETER
Q206=150 ;FEED RATE FOR PLNGN
Q211=0 ;DWELL TIME AT DEPTH
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SETUP CLEARANCE
7 CYCL CALL PAT F5000 M13
8 L Z+100 R0 FMAX
9 TOOL CALL 2 Z S5000
10 L Z+10 R0 F5000
11 CYCL DEF 200 DRILLING
Q200=2 ;SETUP CLEARANCE
Q201=-25 ;DEPTH
Q206=150 ;FEED RATE FOR PECKING
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SETUP CLEARANCE
Q211=0.2 ;DWELL TIME AT DEPTH
12 CYCL CALL PAT F5000 M13
13 L Z+100 R0 FMAX
14 TOOL CALL 3 Z S200
15 L Z+50 R0 FMAX
16 CYCL DEF 206 TAPPING NEW
Q200=2 ;SETUP CLEARANCE
Q201=-25 ;DEPTH OF THREAD
Q206=150 ;FEED RATE FOR PECKING
Q211=0 ;DWELL TIME AT DEPTH
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SETUP CLEARANCE
17 CYCL CALL PAT F5000 M13
18 L Z+100 R0 FMAX M2
19 END PGM 1 MM
104
Cycle definition: CENTERING
Call the cycle in connection with point pattern
Retract the tool, change the tool
Call the drilling tool (radius 2.4)
Move tool to clearance height (enter a value for F)
Cycle definition: drilling
Call the cycle in connection with point 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 point pattern
Retract in the tool axis, end program
Fixed Cycles: Drilling