HEIDENHAIN TNC 620 User Manual page 497

Programming and executing simple machining operations 15.1
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 200 DRILLING.
0 BEGIN PGM $MDI MM
1 TOOL CALL 1 Z S2000
2 L Z+200 R0 FMAX
3 L X+50 Y+50 R0 FMAX M3
4 CYCL DEF 200 DRILLING
Q200=5 ;SET-UP CLEARANCE
Q201=-15 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGNG
Q202=5 ;INFEED DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=-10 ;SURFACE COORDINATE
Q204=20 ;SECOND SET-UP CLEARANCE
Q211=0.2 ;DWELL TIME AT DEPTH
5 CYCL CALL
6 L Z+200 R0 FMAX M2
7 END PGM $MDI MM
Straight-line function: See "Straight line L", page 201
DRILLING cycle: See User's Manual for Cycles, Cycle 200
DRILLING.
TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014
Call the tool: tool axis Z,
spindle speed 2000 rpm
Retract the tool (F MAX = rapid traverse)
Move the tool at F MAX to a position above the hole,
spindle on
Define the DRILLING cycle
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 after every retraction in seconds
Coordinate of the workpiece surface
Set-up clearance of the tool above the hole
Dwell time in seconds at the hole bottom
Call the DRILLING cycle
Retract the tool
End of program
15
497