Cycle Parameters - HEIDENHAIN TNC 620 User Manual

THREAD MILLING (Cycle 262, DIN/ISO: G262, software option 19)

Cycle parameters

Nominal diameter Q335: Nominal thread diameter.
Input range 0 to 99999.9999
Thread pitch Q239: 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
Thread depth Q201 (incremental): Distance
between workpiece surface and root of thread.
Input range -99999.9999 to 99999.9999
Threads per step Q355: 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
Feed rate for pre-positioning Q253: Traversing
speed of the tool when moving in and out of the
workpiece, in mm/min. Input range 0 to 99999.9999
alternatively FMAX, FAUTO
Climb or up-cut Q351: Type of milling operation
with M3
+1
= climb
–1
= up-cut
Set-up clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Input range
0 to 99999.9999
Coordinate of workpiece surface Q203 (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
TNC 620 | User's Manual Cycle Programming | 3/2014
NC blocks
25 CYCL DEF 262 THREAD MILLING
Q335=10 ;NOMINAL DIAMETER
Q239=+1.5 ;THREAD PITCH
Q201=-20 ;THREAD DEPTH
4
4.6
111