HEIDENHAIN TNC 407 (280 580) User Manual User Manual
Page 184
TNC 425/TNC 415 B/TNC 407
6-10
6
Subprograms and Program Section Repeats
Z
X
–3
–15
–20
100
20
20
15
75
Continued...
Cycle definition PECKING for countersinking
Cycle definition PECKING
Cycle definition TAPPING
Tool definition for countersinking (T35), peck drilling (T25) and
tapping (T30)
Example for exercise: Groups of four holes (see page 6-4), and with three different tools
Machining sequence:
Countersinking - Drilling - Tapping
Essential machining data is entered in the fixed
cycle 1: PECK DRILLING (see page 8-5) and
cycle 2: TAPPING (see page 8-7). The tool
moves to the hole groups in a subprogram,
while the machining is performed in a second
subprogram.
Coordinates of the first hole in each group:
1
X = 15 mm
Y = 10 mm
2
X = 45 mm
Y = 60 mm
3
X = 75 mm
Y = 10 mm
Spacing between
holes:
IX = 20 mm
IY = 20 mm
Hole data:
Countersinking
ZC =
3 mm
Ø = 7 mm
Drilling
ZD = 15 mm
Ø = 5 mm
Tapping
ZT = 10 mm
Ø = 6 mm
Part program
0
BEGIN PGM GROUPS2 MM
1
BLK FORM 0.1 Z X+0 Y+0 Z–20
2
BLK FORM 0.2 X+100 Y+100 Z+0
3
TOOL DEF 25 L+0 R+2.5
4
TOOL DEF 30 L+0 R+3
5
TOOL DEF 35 L+0 R+3.5
6
CYCL DEF 1.0 PECKING
7
CYCL DEF 1.1 SET UP–2
8
CYCL DEF 1.2 DEPTH–3
9
CYCL DEF 1.3 PECKG–3 ....................................
10
CYCL DEF 1.4 DWELL0
11
CYCL DEF 1.5 F100
12
TOOL CALL 35 Z S 500
13
CALL LBL 1 ........................................................ Call subprogram 1
14
CYCL DEF 1.0 PECKING
15
CYCL DEF 1.1 SET UP–2
16
CYCL DEF 1.2 DEPTH–25
17
CYCL DEF 1.3 PECKG–6
18
CYCL DEF 1.4 DWELL0
19
CYCL DEF 1.5 F50
20
TOOL CALL 25 Z S 1000
21
CALL LBL 1 ........................................................ Call subprogram 1
22
CYCL DEF 2.0 TAPPING
23
CYCL DEF 2.1 SET UP–2
24
CYCL DEF 2.2 DEPTH–15
25
CYCL DEF 2.3 DWELL0
26
CYCL DEF 2.4 F100
27
TOOL CALL 30 Z S 250
28
CALL LBL 1 ........................................................ Call subprogram 1
29
L Z+100 R0 FMAX M2 ....................................... End program, return to block 1