HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 358)

358 8 Programming: Cycles
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
Point table TAB1.PNT
N100 G79 „PAT“ F5000 M3 * Cycle call in connection with point table TAB1.PNT
Feed rate between points: 5000 mm/min
N110 G00 G40 Z+100 M6 * Retract the tool, change the tool
N120 T2 G17 S5000 * Call tool: drill
N130 G01 G40 Z+10 F5000 * Move tool to clearance height (enter a value for F)
N140 G200 DRILLING Cycle definition: drilling
Q200=2 ;SET-UP CLEARANCE
Q201=-25 ;DEPTH
Q206=150 ;FEED RATE FOR PLNGNG
Q202=5 ;PLUNGING DEPTH
Q210=0 ;DWELL TIME AT TOP
Q203=+0 ;SURFACE COORDINATE 0 must be entered here, effective as defined in point table
Q204=0 ;2ND SET-UP CLEARANCE 0 must be entered here, effective as defined in point table
Q211=0.2 ;DWELL TIME AT DEPTH
N150 G79 “PAT“ F5000 M3 * Cycle call in connection with point table TAB1.PNT
N160 G00 G40 Z+100 M6 * Retract the tool, change the tool
N170 T3 G17 S200 * Tool call for tap
N180 G00 G40 Z+50 * Move tool to clearance height
N190 G84 P01 +2 P02 -15 P03 0 P04 150 * Cycle definition for tapping
N200 G79 “PAT“ F5000 M3 * Cycle call in connection with point table TAB1.PNT
N210 G00 G40 Z+100 M2 * Retract in the tool axis, end program
N99999999 %1 G71 *
TAB1. PNT MM
NR X Y Z
0 +10 +10 +0
1 +40 +30 +0
2 +90 +10 +0
3 +80 +30 +0
4 +80 +65 +0
5 +90 +90 +0
6 +10 +90 +0
7 +20 +55 +0
[END]