HEIDENHAIN iTNC 530 (340 49x-03) - Manual (Page 435)

HEIDENHAIN iTNC 530 435
8.6 SL Cy
cles
ROUGH-OUT (Cycle 22)
1 The TNC positions the tool over the cutter infeed point, taking the
allowance for side into account.
2 In the first plunging depth, the tool mills the contour from the
inside outward at the milling feed rate Q12.
3 The island contours (here: C/D) are cleared out with an approach
toward the pocket contour (here: A/B).
4 In the next step the TNC moves the tool to the next plunging depth
and repeats the roughing procedure until the program depth is
reached.
5 Finally the TNC retracts the tool to the clearance height.
C D
A B
Before programming, note the following:
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)
On pocket contours with pointed inside corners, the use of
an overlap factor greater than 1 can leave residual material.
Use the program verification graphics to inspect the
innermost path especially, and if required, change the
overlap factor slightly. This permits another number of
cutting passes, which often achieves the desired result.