HEIDENHAIN TNC 320 (340 55x-04) Cycle programming - Manual (Page 181)

HEIDENHAIN TNC 320 181
7.
6 R
O
UGH-OUT (Cy
c
le 22, DIN/ISO: G122)
Please note while programming:
This cycle requires a center-cut end mill (ISO 1641) or pilot
drilling with Cycle 21.
You define the plunging behavior of Cycle 22 with
parameter Q19 and with the tool table in the ANGLE and
LCUTS
columns:
„ If Q19=0 is defined, the TNC always plunges
perpendicularly, even if a plunge angle (ANGLE) is defined
for the active tool.
„ If you define the ANGLE=90°, the TNC plunges
perpendicularly. The reciprocation feed rate Q19 is used
as plunging feed rate.
„ If the reciprocation feed rate Q19 is defined in Cycle 22
and ANGLE is defined between 0.1 and 89.999 in the tool
table, the TNC plunges helically at the defined ANGLE.
„ If the reciprocation feed is defined in Cycle 22 and no
ANGLE
is in the tool table, the TNC displays an error
message.
„ If geometrical conditions do not allow helical plunging
(slot geometry), the TNC tries a reciprocating plunge.
The reciprocation length is calculated from LCUTS and
ANGLE
(reciprocation length = LCUTS / tan ANGLE).
If you clear out an acute inside corner and use an overlap
factor greater than 1, some material might be left over.
Check especially the innermost path in the test run graphic
and, if necessary, change the overlap factor slightly. This
allows another distribution of cuts, which often provides
the desired results.
During fine roughing the TNC does not take a defined wear
value DR of the coarse roughing tool into account.