Example: Using Drilling Cycles In Connection With Pattern Def - HEIDENHAIN TNC 640 User Manual

3
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+50 R0 FMAX
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
Q343=0
Q201=-2
Q344=-10
Q206=150
Q211=0
Q203=+0
Q204=10
POSITION 7 GLOBAL DEF 125
Q345=+1
7 CYCL CALL PAT F5000 M13
118
;SET-UP CLEARANCE
;SELECT DIA./DEPTH
;DEPTH
;DIAMETER
;FEED RATE FOR PLNGNG
;DWELL TIME AT DEPTH
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;SELECT POS. HEIGHT
Fixed Cycles: Drilling | Programming Examples
Definition of workpiece blank
Call the centering tool (tool radius 4)
Move tool to clearance height
Define all drilling positions in the point pattern
Cycle definition: CENTERING
With this function the TNC positions to the 2nd set-up
clearance with CYCL CALL PAT between the points. This
function is in effect until M30.
Call the cycle in connection with the hole pattern
HEIDENHAIN | User's manual for cycle programming | 10/2017