HEIDENHAIN TNC 426, User Manual

Page: 242 / 502

216 8 Programming: Cycles
8.3 Cy
cles f
o
r Dr
illing, T
a
pping and Thr
ead Milling
BORING (Cycle 202)
1 The TNC positions the tool in the tool axis at rapid traverse FMAX
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
0° position with an oriented spindle stop.
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 with
FMAX. If Q214=0 the tool point remains on the wall of the hole.
X
Z
Q200
Q201
Q206
Q211
Q203
Q204
Q208
Machine and control must be specially prepared by the
machine tool builder for use of this cycle.
Before programming, note the following:
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.
After the cycle is completed, the TNC restores the coolant
and spindle conditions that were active before the cycle
call.