HEIDENHAIN TNC 620 User Manual page 301

Testing and running | Positioning w/ Manual Data Input operating mode
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
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=-20 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGNG
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=-10 ;SURFACE COORDINATE
Q204=20 ;2ND SET-UP CLEARANCE
Q211=0.2 ;DWELL TIME AT DEPTH
Q395=0 ;DEPTH REFERENCE
5 CYCL CALL
6 L Z+200 R0 FMAX M2
7 END PGM $MDI MM
HEIDENHAIN | TNC 620 | User's Manual for Setup, Testing and Running NC Programs | 01/2022
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 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
Depth referenced to the tool tip or the cylindrical part of the
tool
Call the cycle
Retract the tool
End of program
6
301