HEIDENHAIN TNC 640, User Manual, Page: 800 / 948

Positioning with Manual Data Input | Programming and executing simple machining operations
18
800
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
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
200 DRILLING
.
0 BEGIN PGM $MDI MM
1 TOOL CALL 1 Z S2000
Call the tool: tool axis Z,
spindle speed 2000 rpm
2 L Z+200 R0 FMAX
Retract the tool (F MAX = rapid traverse)
3 L X+50 Y+50 R0 FMAX M3
Move the tool at F MAX to a position above the hole, spindle
on
4 CYCL DEF 200 DRILLING
Define the DRILLING cycle
Q200=5 ;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=5 ;PLUNGING DEPTH
Depth of each infeed before retraction
Q210=0 ;DWELL TIME AT TOP
Dwell time after every retraction in seconds
Q203=-10 ;SURFACE COORDINATE
Coordinate of the workpiece surface
Q204=20 ;2ND SET-UP CLEARANCE
Set-up clearance of the tool above the hole
Q211=0.2 ;DWELL TIME AT DEPTH
Dwell time in seconds at the hole bottom
Q395=0 ;DEPTH REFERENCE
Depth referenced to the tool tip or the cylindrical part of the
tool
5 CYCL CALL
Call the DRILLING cycle
6 L Z+200 R0 FMAX M2
Retract the tool
7 END PGM $MDI MM
End of program
Straight-line function:
Further information: "Straight line L", page 299