Rough-Out (Cycle) - HEIDENHAIN ITNC 530 User Manual

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 inside
outward at the milling feed rate.
3 First the island contours (C and D in the figure at right) are rough-
milled until the pocket contour (A, B) is approached.
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.
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)
406
A
C
Example: NC blocks
59 CYCL DEF 22 ROUGH-OUT
Q10=+5 ;INFEED DEPTH
Q11=100 ;FEED RATE FOR PLUNGING
Q12=350 ;FEED RATE FOR ROUGHING
Q18=1 ;COARSE ROUGHING TOOL
Q19=150 ;RECIPROCATION FEED RATE
Q208=99999 ;RETRACTION FEED RATE
B
D
8 Programming: Cycles