HEIDENHAIN TNC 620 User Manual page 368

9
Programming: Q Parameters
9.13 Programming examples
32 CYCL DEF 10.0 ROTATION
33 CYCL DEF 10.1 ROT+Q8
34 LBL 1
35 CC X+0 Y+0
36 LP PR+Q26 PA+Q8 R0 FQ12
37 CC Z+0 X+Q108
38 L Y+0 Z+0 FQ12
39 LBL 2
40 LP PR+Q6 PA+Q24 FQ12
41 FN 2: Q24 = +Q24 - +Q14
42 FN 11: IF +Q24 GT +Q5 GOTO LBL 2
43 LP PR+Q6 PA+Q5
44 L Z+Q23 R0 F1000
45 L X+Q26 R0 FMAX
46 FN 1: Q28 = +Q28 + +Q18
47 FN 0: Q24 = +Q4
48 CYCL DEF 10.0 ROTATION
49 CYCL DEF 10.0 ROT+Q28
50 FN 12: IF +Q28 LT +Q9 GOTO LBL 1
51 FN 9: IF +Q28 EQU +Q9 GOTO LBL 1
52 CYCL DEF 10.0 ROTATION
53 CYCL DEF 10.1 ROT+0
54 CYCL DEF 7.0 DATUM SHIFT
55 CYCL DEF 7.1 X+0
56 CYCL DEF 7.2 Y+0
57 CYCL DEF 7.3 Z+0
58 LBL 0
59 END PGM SPHERE MM
368
Account for starting angle of rotational position in the plane
Pre-position in the spindle axis
Set pole in the X/Y plane for pre-positioning
Pre-position in the plane
Set pole in the Z/X plane, offset by the tool radius
Move to working depth
Move upward in an approximated "arc"
Update solid angle
Inquire whether an arc is finished. If not finished, return to
LBL 2
Move to the end angle in space
Retract in the spindle axis
Pre-position for next arc
Update rotational position in the plane
Reset solid angle
Activate new rotational position
Unfinished? If not finished, return to LBL 1
Reset the rotation
Reset the datum shift
End of subprogram
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2015