HEIDENHAIN ITNC 530 - CONVERSATIONAL PROGRAMMING User Manual page 581

Example 1
A hole with a depth of 20 mm is to be drilled into a single workpiece.
After clamping and aligning the workpiece and setting the datum, you
can program and execute the drilling operation in a few lines.
First you pre-position the tool with straight-line blocks to the hole
center coordinates at a setup clearance of 5 mm above the workpiece
surface. Then drill the hole with Cycle 200 DRILLING.
0 BEGIN PGM $MDI MM
1 TOOL CALL 1 Z S2000
2 L Z+200 R0 FMAX
3 L X+50 Y+50 R0 FMAX M3
4 CYCL DEF 200 DRILLING
Q200=5 ;SETUP CLEARANCE
Q201=-15 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGN
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=-10 ;SURFACE COORDINATE
Q204=20 ;2ND SETUP CLEARANCE
Q211=0.2 ;DWELL TIME AT DEPTH
5 CYCL CALL
6 L Z+200 R0 FMAX M2
7 END PGM $MDI MM
Straight-line function: See "Straight line L" on page 218, DRILLING
cycle: See User's Manual, Cycles, Cycle 200 DRILLING.
HEIDENHAIN iTNC 530
Call tool: tool axis Z
Spindle speed 2000 rpm
Retract tool (FMAX = rapid traverse)
Move the tool at FMAX to a position above the hole,
spindle on
Define DRILLING cycle
Setup clearance of the tool above the hole
Total hole depth (algebraic sign=working direction)
Feed rate for drilling
Depth of each infeed before retraction
Dwell time after every retraction in seconds
Coordinate of the workpiece surface
Setup clearance of the tool above the hole
Dwell time in seconds at the hole bottom
Call DRILLING cycle
Retract the tool
End of program
581