HEIDENHAIN TNC 410 ISO Programming - Manual (Page 217)

HEIDENHAIN TNC 410, TNC 426, TNC 430 191
8.3 Cy
cles f
o
r Dr
illing
, T
a
p
p
ing
and
Th
read Millin
g UNIVERSAL DRILLING (Cycle G203)
1 The TNC positions the tool in the tool axis at rapid traverse to the
programmed setup clearance above the workpiece surface.
2 The tool drills to the first plunging depth at the programmed feed
rate F.
3 If you have programmed chip breaking, the tool then retracts by
the entered retraction value (with TNC 410: by the set-up
clearance). If you are working without chip breaking, the tool
retracts at the retraction feed rate to set-up clearance, remains
there—if programmed—for the entered dwell time, and advances
again at rapid traverse to the set-up clearance above the first
PLUNGING DEPTH.
4 The tool then advances with another infeed at the programmed
feed rate. If programmed, the plunging depth is decreased after
each infeed by the decrement.
5 The TNC repeats this process (2 to 4) until the programmed total
hole depth is reached.
6 The tool remains at the hole bottom—if programmed—for the
entered dwell time to cut free, and then retracts to set-up
clearance at the retraction feed rate. If you have entered a 2nd set-
up clearance, the tool subsequently moves to that position in rapid
traverse.
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 (tip of drill
taper).
U U U U Feed rate for plunging Q206: Traversing speed of
the tool during drilling in mm/min.
U U U U Plunging depth Q202 (incremental value): Infeed per
cut. The depth does not have to be a multiple of the
plunging depth. The TNC will go to depth in one
movement if:
n
the plunging depth is equal to the depth
n the plunging depth is greater than the depth
U U U U Dwell time at top Q210: Time in seconds that the
tool remains at set-up clearance after having been
retracted from the hole for chip release.
U U U U Workpiece surface coordinate Q203 (absolute
value): Coordinate of the workpiece surface.
Example: NC block
N10 G203 Q200=2 Q201=-20 Q206=150
Q202=5 Q210=0 Q203=+20 Q204=50
Q212=0.2 Q213=3 Q205=3 Q211=0.25
Q208=500 Q256=0.2 *
X
Z
Q200
Q201
Q206
Q202
Q210
Q203
Q204
Q211
Q208
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.