HEIDENHAIN TNC 320 (340 55x-03) - Manual (Page 67)

HEIDENHAIN TNC 320 67
3.1 Pr
ogr
amming and Ex
ecuting
Simple Mac
h
ining Oper
ations
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 in L blocks (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.
Straight line function L, (See “Straight line L” on page 151) DRILLING
cycle. (See “DRILLING (Cycle 200)” on page 217).
Y
X
Z
50
50
0 BEGIN PGM $MDI MM
1 TOOL CALL 1 Z S1860 Call tool: tool axis Z
Spindle speed 1860 rpm
2 L Z+200 R0 FMAX Retract 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 DRILLING cycle
Q200=5 ;SET-UP CLEARANCE Set-up clearance of the tool above the hole
Q201=-15 ;DEPTH Total hole depth (algebraic sign=working direction)
Q206=250 ;FEED RATE FOR PLNGN 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
5 CYCL CALL Call DRILLING cycle
6 L Z+200 R0 FMAX M2 Retract the tool
7 END PGM $MDI MM End of program