HEIDENHAIN iTNC 530 (340 49x-05) Cycle programming - Manual (Page 147)

HEIDENHAIN iTNC 530 147
5.4 SL
O
T
MILLING (Cy
c
le 253, DIN/ISO: G253)
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 (slot position).
The TNC runs the cycle in the axes (machining plane) with
which you approached the starting position. For example,
in X and Y if you programmed CYCL CALL POS X... Y... or
in U and V if you programmed CYCL CALL POS U... V...
The TNC automatically pre-positions the tool in the tool
axis. Note Parameter Q204 (2nd setup clearance).
At the end of the cycle the TNC returns the tool to the
starting point (slot center) 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 setup
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 inside out. You
can therefore mill any slots with small tools, too.
Danger of collision!
Enter in MP7441 bit 2 whether the TNC should output an
error message (bit 2=1) or not (bit 2=0) 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 setup 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: