HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 97)

Programming Examples 3.11
3
TNC 640 | User's Manual Cycle Programming | 5/2013
97
Example: Using drilling cycles in connection with
PATTERN DEF
The drill hole coordinates are stored in the pattern
definition PATTERN DEF POS and are called by the TNC
with CYCL CALL PAT.
The tool radii are selected so that all work steps can be
seen in the test graphics.
Program sequence
Centering (tool radius 4)
Drilling (tool radius 2.4)
Tapping (tool radius 3)
0 BEGIN PGM 1 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
Definition of workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Y+0
3 TOOL CALL 1 Z S5000
Call the centering tool (tool radius 4)
4 L Z+10 R0 F5000 Move tool to clearance height (enter a value for F): the TNC
positions to the clearance height after every cycle
5 PATTERN DEF
Define all drilling positions in the point pattern
POS1( X+10 Y+10 Z+0 )
POS2( X+40 Y+30 Z+0 )
POS3( X+20 Y+55 Z+0 )
POS4( X+10 Y+90 Z+0 )
POS5( X+90 Y+90 Z+0 )
POS6( X+80 Y+65 Z+0 )
POS7( X+80 Y+30 Z+0 )
POS8( X+90 Y+10 Z+0 )
6 CYCL DEF 240 CENTERING
Cycle definition: CENTERING
Q200=2 ;SET-UP CLEARANCE
Q343=0 ;SELECT DEPTH/DIA.
Q201=-2 ;DEPTH
Q344=-10 ;DIAMETER
Q206=150 ;FEED RATE FOR PLNGNG
Q211=0 ;DWELL TIME AT BOTTOM
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
7 CYCL CALL PAT F5000 M13 Call the cycle in connection with the hole pattern
8 L Z+100 R0 FMAX
Retract the tool, change the tool
9 TOOL CALL 2 Z S5000 Call the drilling tool (radius 2.4)
10 L Z+10 R0 F5000 Move tool to clearance height (enter a value for F)
11 CYCL DEF 200 DRILLING
Cycle definition: drilling