HEIDENHAIN TNC 640 User Manual page 183
Hide thumbs
Also See for TNC 640:
- User manual (948 pages) ,
- User manual (903 pages) ,
- Operating instructions manual (64 pages)
Table of Contents
Advertisement
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | RECTANGULAR STUD (Cycle 256, DIN/ISO: G256)
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)
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 while moving 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
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. The overlapping is considered
as maximum overlapping. The overlapping can be
reduced to avoid residual material at the corners.
Input range 0.1 to 1.9999; alternatively PREDEF
HEIDENHAIN | User's manual for cycle programming | 10/2017
NC blocks
8 CYCL DEF 256 RECTANGULAR STUD
Q218=60
;FIRST SIDE LENGTH
Q424=74
;WORKPC. BLANK SIDE 1
Q219=40
;2ND SIDE LENGTH
Q425=60
;WORKPC. BLANK SIDE 2
Q220=5
;CORNER RADIUS
Q368=0.2
;ALLOWANCE FOR SIDE
Q224=+0
;ANGLE OF ROTATION
Q367=0
;STUD POSITION
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
Q437=0
;APPROACH POSITION
Q215=1
;MACHINING OPERATION
Q369=+0
;ALLOWANCE FOR FLOOR
Q338=+0
;INFEED FOR FINISHING
Q385=+0
;FEED RATE FOR
FINISHING
9 L X+50 Y+50 R0 FMAX M3 M99
5
183
Advertisement
Table of Contents
