HEIDENHAIN ITNC 530 User Manual page 415

Milling depth Q1 (incremental value): Distance
between the cylindrical surface and the floor of the
contour.
Finishing allowance for side Q3 (incremental
value): Finishing allowance on the slot wall. The
finishing allowance reduces the slot width by twice
the entered value.
Set-up clearance Q6 (incremental value): Distance
between the tool tip and the cylinder surface.
Plunging depth Q10 (incremental value): Dimension
by which the tool plunges in each infeed.
Feed rate for plunging Q11: Traversing speed of the
tool in the tool axis.
Feed rate for milling Q12: Traversing speed of the
tool in the working plane.
Cylinder radius Q16: Radius of the cylinder on which
the contour is to be machined.
Dimension type ? ang./lin. Q17: The dimensions for
the rotary axis of the subprogram are given either in
degrees (0) or in mm/inches (1).
Slot width Q20: Width of the slot to be machined.
Tolerance? Q21: If you use a tool smaller than the
programmed slot width Q20, process-related
distortion occurs on the slot wall wherever the slot
follows the path of an arc or oblique line. If you define
the tolerance Q21, the TNC adds a subsequent
milling operation to ensure that the slot dimensions
are a close as possible to those of a slot that has been
milled with a tool exactly as wide as the slot. With
Q21 you define the permitted deviation from this
ideal slot. The number of subsequent milling
operations depends on the cylinder radius, the tool
used, and the slot depth. The smaller the tolerance is
defined, the more exact the slot is and the longer the
remachining takes. Recommendation: Use a
tolerance of 0.02 mm
HEIDENHAIN iTNC 530
Example: NC blocks
63 CYCL DEF 28 CYLINDER SURFACE
Q1=-8 ;MILLING DEPTH
Q3=+0 ;ALLOWANCE FOR SIDE
Q6=+0 ;SET-UP CLEARANCE
Q10=+3 ;INFEED DEPTH
Q11=100 ;FEED RATE FOR PLUNGING
Q12=350 ;FEED RATE FOR MILLING
Q16=25 ;RADIUS
Q17=0 ;DIMENSION TYPE
Q20=12 ;SLOT WIDTH
Q21=0 ;TOLERANCE
415