Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling
5.4 SLOT MILLING (Cycle 253, DIN/ISO: G253)
5
144
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
Q206 Feed rate for plunging?: Traversing speed of
the tool in mm/min when plunging to depth. Input
range 0 to 99999.999, alternatively FAUTO, FU, FZ
Q338 Infeed for finishing? (incremental): Infeed in
the spindle axis per finishing cut Q338=0: Finishing
in one infeed. Input range 0 to 99999.9999
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface Input range
0 to 99999.9999; alternatively PREDEF
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
Q204 2nd set-up clearance? (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999; alternatively PREDEF
Q366 Plunging strategy (0/1/2)?: Type of plunging
strategy:
0 = vertical plunging. The plunging angle
(ANGLE) in the tool table is not evaluated.
1, 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.
Alternative: PREDEF
Q385 Finishing feed rate?: Traversing speed of the
tool in mm/min during side and floor finishing. Input
range 0 to 99999.999, alternatively FAUTO, FU, FZ
NC blocks
8 CYCL DEF 253 SLOT MILLING
Q215=0 ;MACHINING
OPERATION
Q218=80 ;SLOT LENGTH
Q219=12 ;SLOT WIDTH
Q368=0.2 ;ALLOWANCE FOR SIDE
Q374=+0 ;ANGLE OF ROTATION
Q367=0 ;SLOT POSITION
Q207=500 ;FEED RATE FOR
MILLNG
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
Q366=1 ;PLUNGE
Q385=500 ;FINISHING FEED RATE
To Next Page
Loading...
