Cycle Parameters - HEIDENHAIN TNC 620 User Manual

3

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
–1
performed)
100
Fixed Cycles: Drilling | BORE MILLING (Cycle 208, software option 19)
= Climb milling
= Up-cut milling (if you enter 0, climb milling is
NC blocks
12 CYCL DEF 208 BORE MILLING
Q200=2
Q201=-80
Q206=150
Q334=1.5
Q203=+100
Q204=50
Q335=25
Q342=0
Q351=+1
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
;SET-UP CLEARANCE
;DEPTH
;FEED RATE FOR PLNGNG
;PLUNGING DEPTH
;SURFACE COORDINATE
;2ND SET-UP CLEARANCE
;NOMINAL DIAMETER
;ROUGHING DIAMETER
;CLIMB OR UP-CUT