Please Note While Programming - HEIDENHAIN TNC 640 User Manual

4
Fixed Cycles: Tapping / Thread Milling | TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206)

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.
For tapping right-hand threads activate the spindle with
M3, for left-hand threads use M4.
It is possible to use the feed rate potentiometer during
tapping. The machine tool builder sets the configuration
(with parameter CfgThreadSpindle>sourceOverride)
for this purpose. The TNC then modifies the speed
accordingly.
The spindle speed potentiometer is inactive.
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.
Danger of collision!
If you enter a positive depth with a cycle, the TNC reverses
calculation of the pre-positioning. This means that the tool
moves at rapid traverse in the tool axis to set-up clearance
below the workpiece surface!
Enter depth as negative
Enter in machine parameter displayDepthErr (No. 201003)
whether the TNC should output an error message (on) or not
(off) if a positive depth is entered
124
NOTICE
HEIDENHAIN | User's manual for cycle programming | 10/2017