Fixed Cycles: Drilling
3.9 BORE MILLING (Cycle 208)
3
86
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
Cycle parameters
Q200 Set-up clearance? (incremental): Distance
between underside of workpiece and the workpiece
top surface. Input range 0 to 99999.9999
Q201 Depth? (incremental): Distance between
workpiece surface and bottom of hole. Input range
-99999.9999 to 99999.9999
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min during helical drilling. Input
range 0 to 99999.999, alternatively FAUTO, FU, FZ
Q334 Feed per revolution of helix (incremental):
Depth of the tool plunge with each helix (=360°).
Input range 0 to 99999.9999
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
Q335 Nominal diameter? (absolute): Bore-hole
diameter. If you have entered the nominal diameter
to be the same as the tool diameter, the TNC will
bore directly to the entered depth without any
helical interpolation. Input range 0 to 99999.9999
Q342 Roughing diameter? (absolute): As soon as
you enter a value greater than 0 in Q342, the TNC
no longer checks the ratio between the nominal
diameter and the tool diameter. This allows you
to rough-mill holes whose diameter is more than
twice as large as the tool diameter. Input range 0 to
99999.9999
Q351 Direction? Climb=+1, Up-cut=-1: Type of
milling operation with M3
+1 = Climb
–1 = Up-cut (if you enter 0, climb milling is
performed)
NC blocks
12 CYCL DEF 208 BORE MILLING
Q200=2 ;SET-UP CLEARANCE
Q201=-80 ;DEPTH
Q206=150 ;FEED RATE FOR
PLNGNG
Q334=1.5 ;PLUNGING DEPTH
Q203=+100;SURFACE COORDINATE
Q204=50 ;2ND SET-UP
CLEARANCE
Q335=25 ;NOMINAL DIAMETER
Q342=0 ;ROUGHING DIAMETER
Q351=+1 ;CLIMB OR UP-CUT
To Next Page
Loading...
