HEIDENHAIN iTNC 530 (60642x-04) Cycle programming - Manual (Page 105)

HEIDENHAIN iTNC 530 105
4.2 T
A
PPING NEW with a Floating
T
a
p Holder (Cy
c
le
206, DIN/ISO:
G206)
4.2 TAPPING NEW with a Floating
Tap Holder (Cycle 206,
DIN/ISO: G206)
Cycle run
1 The TNC positions the tool in the spindle axis at rapid traverse FMAX
to the entered set-up clearance above the workpiece surface.
2 The tool taps to the total hole depth in one movement.
3 Once the tool has reached the total hole depth, the direction of
spindle rotation is reversed and the tool is retracted to the set-up
clearance at the end of the dwell time. If programmed, the tool
moves to the 2nd set-up clearance at FMAX.
4 At the set-up clearance, the direction of spindle rotation reverses
once again.
Please note while programming:
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 DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
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.
If you enter the thread pitch of the tap in the PITCH column
of the tool table, the TNC compares the thread pitch from
the tool table with the thread pitch defined in the cycle.
The TNC displays an error message if the values do not
match. In Cycle 206 the TNC uses the programmed
rotational speed and the feed rate defined in the cycle to
calculate the thread pitch.