HEIDENHAIN iTNC 530 (340 49x-01) ISO programming - Manual (Page 301)

HEIDENHAIN iTNC 530 301
8.4 Cy
cles f
o
r Milling P
o
c
k
ets, St
uds and Slots
8 Path overlap factor Q370: Q370 x tool radius =
Stepover Factor K.
8 Plunging strategy Q366: Type of plunging strategy.
„ 0 = vertical plunging. In the tool table, the plunging
angle ANGLE for the active tool must be defined as
90°. Otherwise the TNC displays an error message.
„ 1 = helical plunging. In the tool table, the plunging
angle ANGLE for the active tool must be defined not
equal to 0. Otherwise the TNC displays an error
message.
„ 2 = reciprocating plunge. In the tool table, the
plunging angle ANGLE for the active tool must be
defined as not equal to 0. The TNC will otherwise
display an error message. The reciprocation length
depends on the plunging angle. As a minimum
value the TNC uses twice the tool diameter.
8 Feed rate for finishing Q385: Traversing speed of
the tool during side and floor finishing in mm/min.
Example: NC blocks
N10 G251 RECTANGULAR POCKET
Q215=0 ;MACHINING OPERATION
Q218=80 ;FIRST SIDE LENGTH
Q219=60 ;SECOND SIDE LENGTH
Q220=5 ;CORNER RADIUS
Q368=0.2 ;ALLOWANCE FOR SIDE
Q224=+0 ;ANGLE OF ROTATION
Q367=0 ;POCKET POSITION
Q207=500 ;FEED RATE FOR MILLING
Q351=+1 ;CLIMB OR UP-CUT
Q201=-20 ;DEPTH
Q202=5 ;PLUNGING DEPTH
Q369=0.1 ;ALLOWANCE FOR FLOOR
Q206=150 ;FEED RATE FOR PLNGNG
Q338=5 ;INFEED FOR FINISHING
Q200=2 ;SET-UP CLEARANCE
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q370=1 ;TOOL PATH OVERLAP
Q366=1 ;PLUNGING
Q385=500 ;FEED RATE FOR FINISHING
N20 G79:G01 X+50 Y+50 Z+0 F15000 M3