HEIDENHAIN TNC 620 User Manual page 166

5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling
5.8 CIRCULAR STUD (cycle 258, DIN/ISO: G258)
Radius/Chamfer Q220: Enter the value for the input
form radius or chamfer. When entering a positive
value between 0 and +99999.9999 the TNC creates
a polygon with round corners. 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.
Finishing allowance for side Q368 (incremental):
Finishing allowance in the working plane. Input
range 0 to 99999.9999
Feed rate for milling Q207: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively FAUTO, FU, FZ
Climb or up-cut Q351: 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 used for
machining)
Depth Q201 (incremental): Distance between
workpiece surface and bottom of stud. Input range
-99999.9999 to 99999.9999
Plunging depth Q202 (incremental): Infeed per
cut. Enter a value greater than 0. Input range 0 to
99999.9999
Feed rate for plunging Q206: Traversing speed of
the tool while moving to depth in mm/min. Input
range 0 to 99999.999; alternatively FMAX, FAUTO,
FU, FZ
166
NC blocks
8 CYCL DEF 258 POLYGON STUDS
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015
Q573=1 ;REFERENCE CIRCUIT
Q571=50 ;REFERENCE CIRCUIT
DIA.
Q222=120 ;WORKPIECE BLANK
DIA.
Q572=10 ;NUMBER OF CORNERS
Q224=40 ;ANGLE OF ROTATION
Q220=2 ;RADIUS/CHAMFER
Q368=0 ;FINISHING
ALLOWANCE FOR SIDE
Q207=3000;FEED RATE FOR
MILLING
Q351=1 ;MILLING TYPE
Q201=-18 ;DEPTH
Q202=10 ;PLUNGING DEPTH
Q206=150 ;FEED RATE FOR
PLUNGING
Q200=2 ;SETUP CLEARANCE
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SETUP
CLEARANCE
Q370=1 ;TOOL PATH OVERLAP