HEIDENHAIN TNC 620 (81760x-02) ISO programming User Manual
Page 497
Programming and executing simple machining operations 15.1
15
TNC 620 | User's ManualDIN/ISO Programming | 2/2015
497
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.
%$MDI G71 *
N10 T1 G17 S2000 *
Call the tool: tool axis Z,
spindle speed 2000 rpm
N20 G00 G40 G90 Z+200 *
Retract the tool (rapid traverse)
N30 X+50 Y+50 M3 *
Move the tool at rapid traverse to a position above the hole.
Spindle on.
N40 G01 Z+2 F2000 *
Position the tool to 2 mm above the hole
N50 G200 *
Define Cycle G200 DRILLING
Q200=2
;SET-UP CLEARANCE
Set-up clearance of the tool above the hole
Q201=-20
;DEPTH
Hole depth (algebraic sign=working direction)
Q206=250
;FEED RATE FOR PLNGNG
Feed rate for drilling
Q202=10
;
Depth of each infeed before retraction
Q210=0
;DWELL TIME AT TOP
Dwell time at top for chip release (in seconds)
Q203=+0
;SURFACE COORDINATE
Workpiece surface coordinate
Q204=50
;2ND SET-UP CLEARANCE
Position after the cycle, with respect to Q203
Q211=0.5
;DWELL TIME AT DEPTH
Dwell time in seconds at the hole bottom
Q395=0
;
Depth referenced to the tool tip or the cylindrical part of the
tool
N60 G79 *
Call Cycle G200 PECKING
N70 G00 G40 Z+200 M2 *
Retract the tool
N9999999 %$MDI G71 *
End of program
Straight-line function: see "Straight line in rapid traverse G00 or
straight line with feed rate F G01", page 217
DRILLING cycle: See User’s Manual, Cycles, Cycle 200 DRILLING.