Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Tapping / Thread Milling | THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264)

Cycle parameters

Q335 Nominal diameter?: Thread nominal
diameter. Input range 0 to 99999.9999
Q239 Pitch?: Pitch of the thread. The algebraic
sign differentiates between right-hand and left-
hand threads:
+ = right-hand thread
–= left-hand thread
Input range -99.9999 to 99.9999
Q201 Depth of thread? (incremental): Distance
between workpiece surface and root of thread.
Input range -99999.9999 to 99999.9999
Q356 Total hole depth? (incremental): Distance
between workpiece surface and bottom of hole.
Input range -99999.9999 to 99999.9999
Q253 Feed rate for pre-positioning?: Traversing
speed of the tool in mm/min when plunging
into the workpiece, or when retracting from
the workpiece. Input range 0 to 99999.9999
alternatively fmax, FAUTO
Q351 Direction? Climb=+1, Up-cut=-1: Type of
milling operation with M3
+1 = Climb milling
–1 = Up-cut milling (if you enter 0, climb milling is
performed)
Q202 Maximum plunging depth? (incremental):
Infeed per cut Q201 DEPTH does not have to be a
multiple of Q202. Input range 0 to 99999.9999
The depth does not have to be a multiple of the
plunging depth. The TNC will go to depth in one
movement if:
the plunging depth is equal to the depth
the plunging depth is greater than the depth
Q258 Upper advanced stop distance?
(incremental): Setup clearance for rapid traverse
positioning when the TNC moves the tool again
to the current plunging depth after retraction from
the hole. Input range 0 to 99999.9999
HEIDENHAIN | User's manual for cycle programming | 10/2017
NC blocks
25 CYCL DEF 264 THREAD DRILLNG/
MLLNG
Q335=10 ;NOMINAL DIAMETER
Q239=+1.5 ;THREAD PITCH
Q201=-16 ;DEPTH OF THREAD
Q356=-20 ;TOTAL HOLE DEPTH
Q253=750 ;F PRE-POSITIONING
Q351=+1 ;CLIMB OR UP-CUT
4
145