HEIDENHAIN TNC 310 (286 140) - Manual (Page 155)

143 HEIDENHAIN TNC 310
Example: Coordinate transformation cycles
Program sequence
■ Program the coordinate transformations in the
main program
■ Program the machining operation in subprogram
1 (see section 9 “Programming: Subprograms and
Program Section Repeats”)
8.6 Cy
cles f
or Coor
dinat
e
T
ransf
or
mations
X
Y
65
65
130
130
45°
X
20
30
10
R5
R5 10
10
Define the workpiece blank
Define the tool
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; execute the milling operation six times
Reset the rotation
Reset the datum shift
Retract in the tool axis, end program
0 BEGIN PGM 11 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+130 Y+130 Z+0
3 TOOL DEF 1 L+0 R+1
4 TOOL CALL 1 Z S4500
5 L Z+250 R0 F MAX
6 CYCL DEF 7.0 DATUM SHIFT
7 CYCL DEF 7.1 X+65
8 CYCL DEF 7.2 Y+65
9 CALL LBL 1
10 LBL 10
11 CYCL DEF 10.0 ROTATION
12 CYCL DEF 10.1 IROT+45
13 CALL LBL 1
14 CALL LBL 10 REP 6/6
15 CYCL DEF 10.0 ROTATION
16 CYCL DEF 10.1 ROT+0
17 CYCL DEF 7.0 DATUM SHIFT
18 CYCL DEF 7.1 X+0
19 CYCL DEF 7.2 Y+0
20 L Z+250 R0 F MAX M2