HEIDENHAIN TNC 640 (34059x-02) ISO programming - Manual (Page 501)

Programming and executing simple machining operations 16.1
16
TNC 640 | User's Manual for DIN/ISO Programming | 5/2013
501
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.
%$MDI G71 *
N10 T1 G17 S2000 *
Call the tool: tool axis Z,
spindle speed 2000 rpm
N20 G00 G40 G90 Z+200 * Retract the tool (rapid traverse)
N30 X+50 Y+50 M3 * Move the tool at rapid traverse to a position above the hole.
Spindle on.
N40 G01 Z+2 F2000 * Position the tool to 2 mm above the hole
N50 G200 DRILLING * Define Cycle G200 DRILLING
Q200=2 ;SET-UP CLEARANCE Set-up clearance of the tool above the hole
Q201=-20 ;DEPTH Hole depth (algebraic sign=working direction)
Q206=250 ;FEED RATE FOR PLNGNG Feed rate for drilling
Q202=10 ;PLUNGING DEPTH Depth of each infeed before retraction
Q210=0 ;DWELL TIME AT TOP Dwell time at top for chip release (in seconds)
Q203=+0 ;SURFACE COORDINATE Workpiece surface coordinate
Q204=50 ;2ND SET-UP CLEARANCE Position after the cycle, with respect to Q203
Q211=0.5 ;DWELL TIME AT BOTTOM Dwell time in seconds at the hole bottom
N60 G79 * Call Cycle G200 PECKING
N70 G00 G40 Z+200 M2 * Retract the tool
N9999999 %$MDI G71 * End of program
Straight-line function: See "Straight line in rapid traverse G00
Straight line with feed rate G01 F", page 197, DRILLING cycle: See
User’s Manual, Cycles, Cycle 200 DRILLING.