HEIDENHAIN TNC 320 (77185x-01) - Manual (Page 465)

Programming and executing simple machining operations 14.1
14
TNC 320 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014
465
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
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=-15 ;DEPTH Hole depth (algebraic sign=working direction)
Q206=250 ;FEED RATE FOR PLNGNG Feed rate for drilling
Q202=5 ;INFEED 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 ;SECOND 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
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: see "Straight line L", page 197
DRILLING cycle: See User’s Manual for Cycles, Cycle 200
DRILLING.