HEIDENHAIN TNC 410 ISO Programming - Manual (Page 255)

HEIDENHAIN TNC 410, TNC 426, TNC 430 229
8.3 Cy
cles f
o
r Dr
illing
, T
a
p
p
ing
and
Th
read Millin
g
Example: Calling drilling cycles in connection with a point table (only with TNC 410)
The drill hole coordinates are stored in the point
table TAB1.PNT and are called by the TNC with
G79 PAT.
The tool radii are selected so that all work steps
can be seen in the test graphics.
Program sequence
n
Centering
n Drilling
n Tapping
%1 G71*
N10 G30 G17 X+0 Y+0 Z-20 * Define the workpiece blank
N20 G31 X+100 Y+100 Z+0 *
N30 G99 1 L+0 R+4 * Tool definition of center drill
N40 G99 2 L+0 R+2.4 * Define tool: drill
N50 G99 3 L+0 R+3 * Tool definition of tap
N60 T1 G17 S5000 * Tool call of centering drill
N70 G01 G40 Z+10 F5000 * Move tool to clearance height (Enter a value for F.
The TNC positions to the clearance height after every cycle)
N80 %:PAT: "TAB1" * Defining point tables
N90 G200 Q200=2 Q201=-2 Q206=150 Q202=2 Cycle definition: Centering
Q210=0 Q203=+0 Q204=0* The value 0 must be entered with Q203 and Q204.
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 the drilling tool
N130 G01 G40 Z+10 F5000 * Move tool to clearance height (enter a value for F)
N140 G200 Q200=2 Q201=-25 Q206=150 Q202=5 Cycle definition: drilling
Q210=0 Q203=+0 Q204=0* The value 0 must be entered with Q203 and Q204.
N150 G79 “PAT“ F5000 M3 * Cycle call in connection with point table TAB1.PNT
X
Y
20
10
100
100
10
90
90 80
30
55
40
65
M6