HEIDENHAIN TNC 640 User Manual page 188

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
188
NC blocks
8 CYCL DEF 257 CIRCULAR STUD
Q223=60 ;FINISHED PART DIA.
Q222=60 ;WORKPIECE BLANK DIA.
Q368=0.2 ;ALLOWANCE FOR SIDE
Q207=500 ;FEED RATE FOR MILLNG
Q351=+1 ;CLIMB OR UP-CUT
Q201=-20 ;DEPTH
Q202=5 ;PLUNGING DEPTH
Q206=150 ;FEED RATE FOR PLNGNG
Q200=2 ;SET-UP CLEARANCE
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP CLEARANCE
Q370=1 ;TOOL PATH OVERLAP
Q376=0 ;STARTING ANGLE
Q215=+1 ;MACHINING OPERATION
Q369=0 ;ALLOWANCE FOR FLOOR
Q338=0 ;INFEED FOR FINISHING
Q385=+500 ;FINISHING FEED RATE
9 L X+50 Y+50 R0 FMAX M3 M99
HEIDENHAIN | User's manual for cycle programming | 10/2017