Please Note While Programming - HEIDENHAIN TNC 320 User's Manual For Cycle Programming

5
CIRCULAR SLOT (Cycle 254, DIN/ISO: G254) 5.5

Please note while programming:

With an inactive tool table you must always plunge
vertically (Q366=0) because you cannot define a
plunging angle.
Pre-position the tool in the machining plane to the
starting position with radius compensation R0. Note
parameter Q367 (position).
The TNC automatically pre-positions the tool in
the tool axis. Pay attention to Q204 2ND SET-UP
CLEARANCE.
At the end of the cycle the TNC returns the tool to
the starting point (center of the pitch circle) in the
working plane. Exception: if you define a slot position
not equal to 0, then the TNC only positions the tool
in the tool axis to the 2nd set-up clearance. In these
cases, always program absolute traverse movements
after the cycle call.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
If the slot width is greater than twice the tool
diameter, the TNC roughs the slot correspondingly
from the inside out. You can therefore mill any slots
with small tools, too.
The slot position 0 is not allowed if you use Cycle
254 Circular Slot in combination with Cycle 221.
The TNC reduces the infeed depth to the LCUTS tool
length defined in the tool table if the tool length is
shorter than the Q202 infeed depth programmed in
the cycle.
Danger of collision!
Enter in machine parameter displayDepthErr
whether the TNC should output an error message
(on) or not (off) if a positive depth is entered.
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 set-up clearance below
the workpiece surface!
If you call the cycle with machining operation 2 (only
finishing), then the TNC positions the tool to the first
plunging depth at rapid traverse!
147
HEIDENHAIN | TNC 320 | User's manual for cycle programming | 9/2016