Back Boring - HEIDENHAIN TNC 320 User Manual

3.7 BACK BORING (Cycle 204,
DIN/ISO: G204)
Cycle run
This cycle allows holes to be bored from the underside of the
workpiece.
1 The TNC positions the tool in the spindle axis at rapid traverse
FMAX to the 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 the 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. Another
oriented spindle stop is carried out and the tool is once again
displaced by the off-center distance.
6 The TNC moves the tool at the pre-positioning feed rate to the set-
up clearance and then—if entered—to the 2nd set-up clearance at
FMAX.
HEIDENHAIN TNC 320 75