HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 169)

153 HEIDENHAIN TNC 410, TNC 426, TNC 430
BACK BORING (Cycle G204)
Machine and TNC must be specially prepared by the
machine tool builder to perform back boring.
Special boring bars for upward cutting are required for
this cycle.
This cycle allows holes to be bored from the underside of the
workpiece.
1 The TNC positions the tool in the tool axis at rapid traverse to set-
up clearance above the workpiece surface.
2 The TNC then orients the spindle to the 0° position
with an oriented spindle stop, and displaces the tool by the off-
center distance.
3 The tool is then plunged into the already bored hole at the feed
rate for pre-positioning until the tooth has reached set-up
clearance on the underside of the workpiece.
4 The TNC then centers the tool again over the bore hole, switches
on the spindle and the coolant and moves at the feed rate for
boring to the depth of bore.
5 If a dwell time is entered, the tool will pause at the top of the
bore hole and will then be retracted from the hole again. The TNC
carries out another oriented spindle stop and the tool is once
again displaced by the off-center distance.
6 The tool then retracts to set-up clearance at the pre-positioning
feed rate, and from there — 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 cycle parameter depth
determines the working direction. Note: A positive sign
bores in the direction of the positive spindle axis.
The entered tool length is the total length to the
underside of the boring bar and not just to the tooth.
When calculating the starting point for boring, the TNC
considers the tooth length of the boring bar and the
thickness of the material.
8.3 Dr
illing Cy
cles
X
Z
Kkap8.pm6 29.06.2006, 08:06 153