HEIDENHAIN TNC 320 User Manual page 540

14
Positioning with Manual Data Input
14.1 Programming and executing simple machining operations
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 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
Q201=-15
Q206=250
Q202=5
Q210=0
Q203=-10
Q204=20
Q211=0.2
Q395=0
5 CYCL CALL
6 L Z+200 R0 FMAX M2
7 END PGM $MDI MM
Straight-line function:
Further Information:
540
;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 L", page 241
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
Depth referenced to the tool tip or the cylindrical part of the
tool
Call the DRILLING cycle
Retract the tool
End of program
HEIDENHAIN | TNC 320 | Conversational Programming User's Manual | 9/2016