Fixed Cycles: Tapping / Thread Milling
4.6 THREAD MILLING (Cycle 262, DIN/ISO: G262)
4
108
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
Cycle parameters
Q335 Nominal diameter?: Thread inside 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
Q355 Number of threads per step?: Number of
thread starts by which the tool is displaced:
0 = one helix on the thread depth
1 = continuous helix on the complete thread length
>1 = several helix paths with approach and
departure, between these the TNC sets the tool by
Q355 x pitch. Input range 0 to 99999
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
–1 = Up-cut (if you enter 0, climb milling is
performed)
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface Input range
0 to 99999.9999
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
NC blocks
25 CYCL DEF 262 THREAD MILLING
Q335=10 ;NOMINAL DIAMETER
Q239=+1.5 ;THREAD PITCH
Q201=-20 ;DEPTH OF THREAD
Q355=0 ;THREADS PER STEP
To Next Page
Loading...
