Cycle Parameters - HEIDENHAIN TNC 640 User Manual

5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | POLYGON STUD (Cycle 258, DIN/ISO: G258)

Cycle parameters

Q573 Inscr.circle/circumcircle (0/1)?: Definition
of whether the dimensioning shall reference to the
inscribed circle or to the perimeter:
0= dimensioning refers to the inscribed circle
1= dimensioning refers to the perimeter
Q571 Reference circle diameter?: Definition of
the diameter of the reference circle. Specify in
parameter Q573 whether the diameter references
to the inscribed circle or the perimeter. Input range
0 to 99999.9999
Q222 Workpiece blank diameter?: Definition
of the diameter of the workpiece blank. The
workpiece blank diameter must be greater than
the reference circle diameter. The TNC performs
multiple stepovers if the difference between the
workpiece blank diameter and reference circle
diameter is greater than the permitted stepover
(tool radius multiplied by path overlap Q370). The
TNC always calculates a constant stepover. Input
range 0 to 99999.9999
Q572 Number of corners?: Enter the number
of corners of the polygon. The TNC will always
equally divide the corners on the stud. Input range
3 to 30
Q224 Angle of rotation?: Specify which angle is
used to machine the first corner of the polygon.
Input range: -360° to +360°
Q220 Radius / Chamfer (+/-)?: Enter the value
for the input form radius or chamfer. If you enter
a positive value between 0 and +99999.9999,
the TNC rounds every corner. The radius refers
to the value you entered. If you enter a negative
value between 0 and -99999.9999 all corners of
the contour are chamfered and the value entered
refers to the length of the chamfer.
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. (If
you enter a negative value, the TNC repositions
the tool after roughing to a diameter outside
of the workpiece blank diameter.) Input range
-99999.9999 to 99999.9999
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively FAUTO, fu, FZ
Q351 Direction? Climb=+1, Up-cut=-1: Type of
milling operation with M3:
+1 = Climb
–1 = Up-cut
PREDEF: The TNC uses the value from the
GLOBAL DEF block (if you enter 0, climb milling is
performed)
192
NC blocks
8 CYCL DEF 258 POLYGON STUD
Q573=1 ;REFERENCE CIRCLE
Q571=50 ;REF-CIRCLE DIAMETER
Q222=120 ;WORKPIECE BLANK DIA.
Q572=10 ;NUMBER OF CORNERS
Q224=40 ;ANGLE OF ROTATION
Q220=2 ;RADIUS / CHAMFER
Q368=0 ;ALLOWANCE FOR SIDE
Q207=3000 ;FEED RATE FOR MILLNG
Q351=1 ;CLIMB OR UP-CUT
Q201=-18 ;DEPTH
Q202=10 ;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
HEIDENHAIN | User's manual for cycle programming | 10/2017