HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 164)

8 Programming: Cycles 148
DRILLING (Cycle G200)
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 first plunging depth at the programmed feed
rate F.
3 The TNC returns the tool at rapid traverse to the setup clearance,
dwells there (if a dwell time was entered), and then moves at
rapid traverse to the setup clearance above the first plunging
depth.
4 The tool then advances with another infeed at the programmed
feed rate F.
5 The TNC repeats this process (2 to 4) until the programmed total
hole depth is reached.
6 At the hole bottom, the tool path is retraced to set-up clearance
or, if programmed, to the 2nd set-up clearance in rapid traverse.
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 depth parameter determines
the working direction.
ú Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface. Enter a
positive value.
ú Depth Q201 (incremental value): Distance between
workpiece surface and bottom of hole (tip of drill
taper)
ú Feed rate for plunging Q206: Traversing speed of the
tool during drilling in mm/min
ú Plunging depth Q202 (incremental value):
Infeed per cut The TNC will go to depth in one
movement if:
■ the plunging depth is equal to the depth
■ the plunging depth is greater than the depth
The depth does not have to be a multiple of the
plunging depth.
ú 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remains at set-up clearance after having been
retracted from the hole for chip release.
ú Workpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface
X
Z
Q200
Q201
Q206
Q202
Q210
Q203
Q204
8.3 Dr
illing Cy
cles
Example NC block:
N70 G200 Q200=2 Q201=-20 Q206=150
Q202=5 Q210=0 Q203=+0 Q204=50*
Kkap8.pm6 29.06.2006, 08:06 148