Example: Using Drilling Cycles In Connection With Pattern Def - HEIDENHAIN TNC 320 User's Manual For Cycle Programming

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
2 BLK FORM 0.2 X+100 Y+100 Y+0
3 TOOL CALL 1 Z S5000
4 L Z+10 R0 F5000
5 PATTERN DEF
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
Q200=2 ;SET-UP CLEARANCE
Q343=0 ;SELECT DIA./DEPTH
Q201=-2 ;DEPTH
Q344=-10 ;DIAMETER
Q206=150 ;FEED RATE FOR PLNGNG
Q211=0 ;DWELL TIME AT DEPTH
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
7 CYCL CALL PAT F5000 M13
8 L Z+100 R0 FMAX
9 TOOL CALL 2 Z S5000
10 L Z+10 R0 F5000
HEIDENHAIN | TNC 320 | User's manual for cycle programming | 9/2016
Programming Examples 3.11
Definition of workpiece blank
Call the centering tool (tool radius 4)
Move tool to clearance height (enter a value for F): the TNC
positions to the clearance height after every cycle
Define all drilling positions in the point pattern
Cycle definition: CENTERING
Call the cycle in connection with the hole pattern
Retract the tool, change the tool
Call the drilling tool (radius 2.4)
Move tool to clearance height (enter a value for F)
3
91