HEIDENHAIN TNC 640 User Manual page 750

18
Positioning with Manual Data Input | Programming and executing simple machining operations
Example
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 preset, you can program and execute the drilling operation with
a few lines of programming.
First you pre-position the tool above the workpiece with straight-
line blocks and position with a safety clearance of 5 mm above the
hole. Then drill the hole with Cycle G200.
%$MDI G71 *
N10 T1 G17 S2000*
N20 G00 G40 G90 Z+200*
N30 X+50 Y+50 M3*
N40 G01 Z+2 F2000*
N50 G200 DRILLING
Q200=2
Q201=-20
Q206=250
Q202=10
Q210=0
Q203=+0
Q204=50
Q211=0.5
Q395=0
N60 G79*
N70 G00 G40 Z+200 M2*
N9999999 %$MDI G71 *
Straight-line function:
Further information:
line with feed rate F G01", page 295
750
;SET-UP CLEARANCE
;DEPTH
;FEED RATE FOR PLNGNG
;PLUNGING DEPTH
;DWELL TIME AT TOP
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;DWELL TIME AT DEPTH
;DEPTH REFERENCE
"Straight line in rapid traverse G00 or straight
Call the tool: tool axis Z,
spindle speed 2000 rpm
Retract the tool (rapid traverse)
Move the tool at rapid traverse to a position above the hole.
Spindle on.
Position the tool to 2 mm above the hole
Define Cycle G200 DRILLING
Set-up clearance of the tool above the hole
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
Depth referenced to the tool tip or the cylindrical part of the
tool
Call Cycle G200 PECKING
Retract the tool
End of program
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017