HEIDENHAIN iTNC 530 (340 420) ISO programming - Manual (Page 229)

HEIDENHAIN iTNC 530 229
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
BORING (Cycle G202)
1 The TNC positions the tool in the tool axis at rapid traverse to the
set-up clearance above the workpiece surface.
2 The tool drills to the programmed depth at the feed rate for
plunging.
3 If programmed, the tool remains at the hole bottom for the entered
dwell time with active spindle rotation for cutting free.
4 The TNC then orients the spindle to the position that is defined in
parameter Q336.
5 If retraction is selected, the tool retracts in the programmed
direction by 0.2 mm (fixed value).
6 The TNC moves the tool at the retraction feed rate to the set-up
clearance and then, if entered, to the 2nd set-up clearance at rapid
traverse. If Q214=0 the tool point remains on the wall of the hole. X
Z
Q200
Q201
Q206
Q211
Q203
Q204
Q208
The TNC and the machine tool must be specially prepared
by the machine tool builder for the use of Cycle G202.
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation G40.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH = 0, the cycle will not be executed.
After the cycle is completed, the TNC restores the coolant
and spindle conditions that were active before the cycle
call.
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.
Danger of collision!
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
at safety clearance below the workpiece surface!