HEIDENHAIN ITNC 530 User Manual page 374

Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
Depth Q201 (incremental value): Distance between
workpiece surface and bottom of pocket.
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 value lower
than that defined in Q207.
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 pocket in the reference axis of the working plane.
Center in 2nd axis Q217 (absolute value): Center of
the pocket in the minor axis of the working plane.
1st side length Q218 (incremental value): Pocket
length, parallel to the reference axis of the working
plane.
2nd side length Q219 (incremental value): Pocket
length, parallel to the minor axis of the working plane.
Corner radius Q220: Radius of the pocket corner: If
you make no entry here, the TNC assumes that the
corner radius is equal to the tool radius.
Allowance in 1st axis Q221 (incremental value):
Allowance for pre-positioning in the reference axis of
the working plane referenced to the length of the
pocket.
374
Example: NC blocks
354 CYCL DEF 212 POCKET 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
Q218=80 ;1ST SIDE LENGTH
Q219=60 ;2ND SIDE LENGTH
Q220=5 ;CORNER RADIUS
Q221=0 ;OVERSIZE
8 Programming: Cycles