HEIDENHAIN TNC 620 (81760x-01) Cycle programming - Manual (Page 273)

Programming Examples 11.10
11
TNC 620 | User's Manual Cycle Programming | 3/2014
273
11.10 Programming Examples
Example: Coordinate transformation cycles
Program sequence
Program the coordinate transformations in the main
program
Machining within a subprogram
0 BEGIN PGM COTRANS MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
Definition of workpiece blank
2 BLK FORM 0.2 X+130 Y+130 Z+0
3 TOOL CALL 1 Z S4500
Tool call
4 L Z+250 R0 FMAX Retract the tool
5 CYCL DEF 7.0 DATUM SHIFT
Shift datum to center
6 CYCL DEF 7.1 X+65
7 CYCL DEF 7.2 Y+65
8 CALL LBL 1
Call milling operation
9 LBL 10 Set label for program section repeat
10 CYCL DEF 10.0 ROTATION Rotate by 45° (incremental)
11 CYCL DEF 10.1 IROT+45
12 CALL LBL 1
Call milling operation
13 CALL LBL 10 REP 6/6
Return jump to LBL 10; repeat the milling operation six
times
14 CYCL DEF 10.0 ROTATION Reset the rotation
15 CYCL DEF 10.1 ROT+0
16 CYCL DEF 7.0 DATUM SHIFT
Reset the datum shift
17 CYCL DEF 7.1 X+0
18 CYCL DEF 7.2 Y+0
19 L Z+250 R0 FMAX M2
Retract in the tool axis, end program
20 LBL 1 Subprogram 1
21 L X+0 Y+0 R0 FMAX Define milling operation
22 L Z+2 R0 FMAX M3
23 L Z-5 R0 F200
24 L X+30 RL
25 L IY+10
26 RND R5
27 L IX+20
28 L IX+10 IY-10