HEIDENHAIN TNC 620 User Manual page 180

5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | CIRCULAR STUD (Cycle 257, DIN/ISO: G257,
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
Q370 Path overlap factor?: Q370 x tool radius =
stepover factor k. Input range: 0.0001 to 1.9999
alternatively PREDEF
Q376 Starting angle?: Polar angle relative to the
stud center from which the tool approaches the
stud. Input range 0 to 359°
Q215 Machining operation (0/1/2)?: Define the
extent of machining:
0: Roughing and finishing
1: Roughing only
2: Finishing only
Q369 Finishing allowance for floor?
(incremental): Finishing allowance for the floor.
Input range 0 to 99999.9999
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
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
180
NC blocks
8 CYCL DEF 257 CIRCULAR STUD
Q223=60
Q222=60
Q368=0.2
Q207=500
Q351=+1
Q201=-20
Q202=5
Q206=150
Q200=2
Q203=+0
Q204=50
Q370=1
Q376=0
Q215=+1
Q369=0
Q338=0
Q385=+500
9 L X+50 Y+50 R0 FMAX M3 M99
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
software option 19)
;FINISHED PART DIA.
;WORKPIECE BLANK DIA.
;ALLOWANCE FOR SIDE
;FEED RATE FOR MILLNG
;CLIMB OR UP-CUT
;DEPTH
;PLUNGING DEPTH
;FEED RATE FOR PLNGNG
;SET-UP CLEARANCE
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;TOOL PATH OVERLAP
;STARTING ANGLE
;MACHINING OPERATION
;ALLOWANCE FOR FLOOR
;INFEED FOR FINISHING
;FINISHING FEED RATE