HEIDENHAIN iTNC 530 User Manual page 523

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 G200.
%$MDI G71 *
N10 T1 G17 S2000 *
N20 G00 G40 G90 Z+200 *
N30 X+50 Y+50 M3 *
N40 G01 Z+2 F2000 *
N50 G200 DRILLING *
Q200=2 ;SETUP CLEARANCE
Q201=-20 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGN
Q202=10 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SETUP CLEARANCE
Q211=0.5 ;DWELL TIME AT DEPTH
N60 G79 *
N70 G00 G40 Z+200 M2 *
N9999999 %$MDI G71 *
Straight-line function: See "Straight line at rapid traverse G00 Straight
line with feed rate G01 F" on page 217, DRILLING cycle: See User's
Manual, Cycles, Cycle 200 DRILLING.
HEIDENHAIN iTNC 530
Call tool: tool axis Z
Spindle speed 2000 rpm
Retract tool (rapid traverse)
Move the tool at rapid traverse to a position above
the hole,
spindle on
Position tool to 2 mm above hole
Define Cycle G200 Drilling
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 at top for chip release (in seconds)
Workpiece surface coordinate
Position after the cycle, with respect to Q203
Dwell time in seconds at the hole bottom
Call Cycle G200 PECKING
Retract the tool
End of program
523