HEIDENHAIN TNC 410 ISO Programming - Manual (Page 215)

HEIDENHAIN TNC 410, TNC 426, TNC 430 189
8.3 Cy
cles f
o
r Dr
illing
, T
a
p
p
ing
and
Th
read Millin
g BORING (Cycle G202)
1 The TNC positions the tool in the tool axis at rapid traverse to the
setup 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 at rapid
traverse. If Q214=0, the tool point remains on the wall of the hole.
U U U U Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
U U U U Depth Q201 (incremental value): Distance between
workpiece surface and bottom of hole.
U U U U Feed rate for plunging Q206: Traversing speed of
the tool during boring in mm/min.
U U U U Dwell time at depth Q211: Time in seconds that the
tool remains at the hole bottom.
U U U U Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting from the hole. If you
enter Q208 = 0, the tool retracts at feed rate for
plunging.
U U U U Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface.
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.
Example: NC block
N90 G202 Q200=2 Q201=-20 Q206=150
Q211=0 Q208=30000 Q203=+0 Q204=50
Q214=0 Q336=0 *