HEIDENHAIN TNC 426, User Manual

Page: 420 / 502

394 10 Programming: Q Parameters
1
0
.1
1 Pr
ogr
amming Examples
20 CALL LBL 10 Call machining operation
21 L Z+100 R0 F MAX M2
Retract in the tool axis, end program
22 LBL 10
Subprogram 10: Machining operation
23 Q16 = Q6 - Q10 - Q108 Account for allowance and tool, based on the cylinder radius
24 FN 0: Q20 = +1
Set counter
25 FN 0: Q24 = +Q4 Copy starting angle in space (Z/X plane)
26 Q25 = (Q5 - Q4) / Q13
Calculate angle increment
27 CYCL DEF 7.0 DATUM SHIFT Shift datum to center of cylinder (X axis)
28 CYCL DEF 7.1 X+Q1
29 CYCL DEF 7.2 Y+Q2
30 CYCL DEF 7.3 Z+Q3
31 CYCL DEF 10.0 DREHUNG Account for rotational position in the plane
32 CYCL DEF 10.1 ROT+Q8
33 L X+0 Y+0 R0 F MAX Pre-position in the plane to the cylinder center
34 L Z+5 R0 F1000 M3
Pre-position in the tool axis
35 LBL 1
36 CC Z+0 X+0
Set pole in the Z/X plane
37 LP PR+Q16 PA+Q24 FQ11 Move to starting position on cylinder, plunge-cutting obliquely into
38 L Y+Q7 R0 FQ12
Longitudinal cut in Y+ direction
39 FN 1: Q20 = +Q20 + +1 Update the counter
40 FN 1: Q24 = +Q24 + +Q25
Update solid angle
41 FN 11: IF +Q20 GT +Q13 GOTO LBL 99 Finished? If finished, jump to end.
42 LP PR+Q16 PA+Q24 FQ11
Move in an approximated “arc” for the next longitudinal cut.
43 L Y+0 R0 FQ12 Longitudinal cut in Y– direction
44 FN 1: Q20 = +Q20 + +1
Update the counter
45 FN 1: Q24 = +Q24 + +Q25 Update solid angle
46 FN 12: IF +Q20 LT +Q13 GOTO LBL 1
Unfinished? If not finished, return to LBL 1
47 LBL 99
48 CYCL DEF 10.0 DREHUNG
Reset the rotation
49 CYCL DEF 10.1 ROT+0
50 CYCL DEF 7.0 DATUM SHIFT
Reset the datum shift
51 CYCL DEF 7.1 X+0
52 CYCL DEF 7.2 Y+0
53 CYCL DEF 7.3 Z+0
54 LBL 0
End of subprogram
55 END PGM CYLIN MM