HEIDENHAIN ITNC 530 User Manual page 362

Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
Workpiece surface coordinate Q203 (absolute
value): Absolute coordinate of the workpiece surface
2nd set-up clearance Q204 (incremental value):
Coordinate in the tool axis at which no collision
between tool and workpiece (clamping devices) can
occur.
Path overlap factor Q370: Q370 x tool radius =
stepover factor k.
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.
Feed rate for finishing Q385: Traversing speed of
the tool during side and floor finishing in mm/min.
362
Example: NC blocks
8 CYCL DEF 252 CIRCULAR POCKET
Q215=0 ;MACHINING OPERATION
Q223=60 ;CIRCLE DIAMETER
Q368=0.2 ;ALLOWANCE FOR SIDE
Q207=500 ;FEED RATE FOR MILLING
Q351=+1 ;CLIMB OR UP-CUT
Q201=-20 ;DEPTH
Q202=5 ;INFEED 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
9 CYCL CALL POS X+50 Y+50 Z+0 FMAX M3
8 Programming: Cycles