HEIDENHAIN TNC 310 (286 140) - Manual (Page 117)

105 HEIDENHAIN TNC 310
TAPPING with a floating tap holder (Cycle 2)
1 The tool drills to the total hole depth in one movement
2 Once the tool has reached the total hole depth, the direction of
spindle rotation is reversed and the tool is retracted to the
starting position at the end of the DWELL TIME.
3 At the starting position, the direction of spindle rotation reverses
once again.
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with RADIUS
COMPENSATION R0.
Program a positioning block for the starting point in the
tool axis (set-up clearance above the workpiece surface).
The algebraic sign for the depth parameter determines
the working direction.
A floating tap holder is required for tapping. It must
compensate the tolerances between feed rate and
spindle speed during the tapping process.
When a cycle is being run, the spindle speed override
knob is disabled. The feed rate override knob is active
only within a limited range, which is defined by the
machine tool builder (refer to your machine manual).
For tapping right-hand threads activate the spindle with
M3, for left-hand threads use M4.
ú Setup clearance (incremental value): Distance
between tool tip (at starting position) and
workpiece surface. Standard value: approx. 4 times
the thread pitch
ú Total hole depth (thread length, incremental
value): Distance between workpiece surface and
end of thread
ú Dwell time in seconds: Enter a value between 0
and 0.5 seconds to avoid wedging of the tool
during retraction.
ú Feed rate F: Traversing speed of the tool during
tapping
The feed rate is calculated as follows: F = S x p,
where
F is the feed rate in mm/min),
S is the spindle speed in rpm,
and p is the thread pitch in mm
8.2 Dr
illing Cy
cles
X
Z