HEIDENHAIN TNC 320 (340 55x-04) Cycle programming - Manual (Page 93)

HEIDENHAIN TNC 320 93
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 to the entered setup
clearance above the workpiece surface at rapid traverse FMAX.
2 The tool drills 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 setup
clearance at the end of the dwell time. If programmed, the tool
moves to the 2nd setup clearance at FMAX.
4 At the setup 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.
Danger of collision!
Use the machine parameter displayDepthErr to define
whether, if a positive depth is entered, the TNC should
output an error message (on) or not (off).
Keep in mind that the TNC reverses the calculation for pre-
positioning when a positive depth is entered. This
means that the tool moves at rapid traverse in the tool axis
to setup clearance below the workpiece surface!