Programming Examples; Example: Coordinate Transformation Cycles - HEIDENHAIN TNC 620 User Manual

10

10.10 Programming Examples

Example: Coordinate transformation cycles

Program run
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
2 BLK FORM 0.2 X+130 X+130 Z+0
3 TOOL CALL 1 Z S4500
4 L Z+250 R0 FMAX
5 CYCL DEF 7.0 DATUM SHIFT
6 CYCL DEF 7.1 X+65
7 CYCL DEF 7.2 Y+65
8 CALL LBL 1
9 LBL 10
10 CYCL DEF 10.0 ROTATION
11 CYCL DEF 10.1 IROT+45
12 CALL LBL 1
13 CALL LBL 10 REP 6/6
14 CYCL DEF 10.0 ROTATION
15 CYCL DEF 10.1 ROT+0
16 CYCL DEF 7.0 DATUM SHIFT
17 CYCL DEF 7.1 X+0
18 CYCL DEF 7.2 Y+0
19 L Z+250 R0 FMAX M2
20 LBL 1
21 L X+0 Y+0 R0 FMAX
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
306
Cycles: Coordinate Transformations | Programming Examples
Definition of workpiece blank
Tool call
Retract the tool
Shift datum to center
Call milling operation
Set label for program section repeat
Rotate by 45° (incremental)
Call milling operation
Return jump to LBL 10; repeat the milling operation six times
Reset the rotation
Reset the datum shift
Retract in the tool axis, end program
Subprogram 1
Define milling operation
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017