Table of Contents
Advertisement
5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling
5.8
POLYGON STUD (Cycle 258, DIN/ISO: G258)
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 of the polygon stud. 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 Input
range 0 to 99999.9999
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min during 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)
Q201 Depth? (incremental): Distance between
workpiece surface and bottom of stud. Input range
-99999.9999 to 99999.9999
Q202 Plunging depth? (incremental): Infeed per
cut; enter a value greater than 0. Input range 0 to
99999.9999
Q206 Feed rate for plunging?: Traversing speed of
the tool in mm/min when plunging to depth. Input
range 0 to 99999.999; alternatively FMAX, FAUTO,
FU, FZ
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
162
NC blocks
8 CYCL DEF 258 POLYGON STUD
9 L X+50 Y+50 R0 FMAX M3 M99
HEIDENHAIN | TNC 320 | User's manual for cycle programming | 9/2016
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
Q215=0
;MACHINING
OPERATION
Q369=0
;ALLOWANCE FOR
FLOOR
Q338=0
;INFEED FOR FINISHING
Q385=500
;FINISHING FEED RATE
Advertisement
Table of Contents
