HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 262)

262 8 Programming: Cycles
8.5 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.
8 Plunging depth Q10 (incremental value): Dimension
by which the tool plunges in each infeed.
8 Feed rate for plunging Q11: Traversing speed of the
tool in mm/min during penetration.
8 Feed rate for milling Q12: Traversing speed for
milling in mm/min.
Example: NC blocks
59 CYCL DEF 22 ROUGH-OUT
Q10=+5 ;PLUNGING 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
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 on a zigzag path 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.