HEIDENHAIN ITNC 530 User Manual page 380

Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
Depth Q201 (incremental value): Distance between
workpiece surface and bottom of stud.
Feed rate for plunging Q206: Traversing speed of
the tool in mm/min when moving to depth. If you are
plunge-cutting into the material, enter a low value; if
you have already cleared the stud, enter a higher feed
rate.
Plunging depth Q202 (incremental value): Infeed per
cut. Enter a value greater than 0.
Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface.
2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices) can
occur.
Center in 1st axis Q216 (absolute value): Center of
the stud in the reference axis of the working plane.
Center in 2nd axis Q217 (absolute value): Center of
the stud in the minor axis of the working plane.
Workpiece blank diameter Q222: Diameter of the
premachined stud for calculating the pre-position.
Enter the workpiece blank diameter to be greater
than the diameter of the finished part.
Diameter of finished part Q223: Diameter of the
finished stud. Enter the diameter of the finished part
to be less than the workpiece blank diameter.
380
Example: NC blocks
43 CYCL DEF 215 C. STUD FINISHING
Q200=2 ;SET-UP CLEARANCE
Q201=-20 ;DEPTH
Q206=150 ;FEED RATE FOR PLUNGING
Q202=5 ;INFEED DEPTH
Q207=500 ;FEED RATE FOR MILLING
Q203=+30 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q216=+50 ;CENTER IN 1ST AXIS
Q217=+50 ;CENTER IN 2ND AXIS
Q222=81 ;WORKPIECE BLANK DIA.
Q223=80 ;FINISHED PART DIA.
8 Programming: Cycles