HEIDENHAIN TNC 310 (286 140) - Manual (Page 114)

8 Programming: Cycles 102
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with RADIUS
COMPENSATION R0.
The algebraic sign for the cycle parameter TOTAL HOLE
DEPTH determines the working direction.
ú Set-up clearance Q200 (incremental value):
Distance between tool tip and workpiece surface.
ú Depth Q201 (incremental value): Distance between
workpiece surface and bottom of hole (tip of drill
taper)
ú Feed rate for plunging Q206: Traversing speed of
the tool during drilling in mm/min
ú Plunging depth Q202 (incremental value):
Infeed per cut The TNC will go to depth in one
movement if:
■ the plunging depth is equal to the depth
■ the plunging depth is greater than the depth
The depth does not have to be a multiple of the
plunging depth.
ú Dwell time at top Q210: Time in seconds that the
tool remains at set-up clearance after having been
retracted from the hole for chip release.
ú Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface
ú 2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices)
can occur.
ú Decrement Q212 (incremental value): Value by
which the TNC decreases the plunging depth after
each infeed.
ú Nr of breaks before retracting Q213: Number of
chip breaks after which the TNC is to withdraw the
tool from the hole for chip release. For chip
breaking, the TNC retracts the tool each time
by 0.2 mm.
ú Minimum plunging depth Q205 (incremental
value): If you have entered a decrement, the TNC
limits the plunging depth to the value entered with
Q205.
ú Dwell time at depth Q211: Time in seconds that
the tool remains at the hole bottom
ú Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting from the hole. If
you enter Q208 = 0, the tool retracts in FMAX.
X
Z
Q200
Q201
Q206
Q202
Q210
Q203
Q204
Q211
Q208
8.2 Dr
illing Cy
cles