HEIDENHAIN TNC 620 (73498x-01) ISO programming - Manual (Page 387)

HEIDENHAIN TNC 620 387
14.1 Pr
ogr
amming and ex
ecuting simple mac
h
ining oper
ations
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.
Straight-line function: See "Straight line at rapid traverse G00 Straight
line with feed rate G01 F" on page 174, DRILLING cycle: See User’s
Manual, Cycles, Cycle 200 DRILLING.
%$MDI G71 *
N10 T1 G17 S2000 * Call tool: tool axis Z
Spindle speed 2000 rpm
N20 G00 G40 G90 Z+200 * Retract tool (rapid traverse)
N30 X+50 Y+50 M3 * Move the tool at rapid traverse to a position above
the hole,
Spindle on
N40 G01 Z+2 F2000 * Position tool to 2 mm above hole
N50 G200 DRILLING * Define Cycle G200 Drilling
Q200=2 ;SET-UP CLEARANCE Set-up clearance of the tool above the hole
Q201=-20 ;DEPTH Total hole depth (algebraic sign=working direction)
Q206=250 ;FEED RATE FOR PLNGN Feed rate for drilling
Q202=10 ;PLUNGING DEPTH Depth of each infeed before retraction
Q210=0 ;DWELL TIME AT TOP Dwell time at top for chip release (in seconds)
Q203=+0 ;SURFACE COORDINATE Workpiece surface coordinate
Q204=50 ;2ND SET-UP CLEARANCE Position after the cycle, with respect to Q203
Q211=0.5 ;DWELL TIME AT DEPTH Dwell time in seconds at the hole bottom
N60 G79 * Call Cycle G200 PECKING
N70 G00 G40 Z+200 M2 * Retract the tool
N9999999 %$MDI G71 * End of program