HEIDENHAIN iTNC 530 (60642x-04) Cycle programming - Manual (Page 75)

HEIDENHAIN iTNC 530 75
3.4 REAMING (Cy
c
le
20
1, DIN/ISO:
G20
1
)
3.4 REAMING (Cycle 201,
DIN/ISO: G201)
Cycle run
1 The TNC positions the tool in the spindle axis at rapid traverse FMAX
to the entered set-up clearance above the workpiece surface.
2 The tool reams to the entered depth at the programmed feed
rate F.
3 If programmed, the tool remains at the hole bottom for the entered
dwell time.
4 The tool then retracts to the set-up clearance at the feed rate F,
and from there—if programmed—to the 2nd set-up clearance at
FMAX
.
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.
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 set-up clearance below the workpiece surface!
Enter in MP7441 bit 0 whether the TNC should output an
error message (bit 0=0) or not (bit 0=1) if spindle rotation
is not active when the cycle is called. The function also
needs to be adapted by your machine manufacturer.