Please Note While Programming - HEIDENHAIN TNC 620 User Manual

5
SLOT MILLING (Cycle 253, DIN/ISO: G253) 5.4

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. Note the 2nd set-up clearance Q204.
At the end of the cycle the TNC merely moves the
tool in working plane back to the center of the slot;
in the other working plane axis the TNC does not do
any positioning. 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. Prior to a new cycle
call, move the tool back to the starting position or
program always absolute traverse motions 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 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!
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 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 620 | User's manual for cycle programming | 9/2015