HEIDENHAIN TNC 320 (340 55x-04) Cycle programming - Manual (Page 100)

100 Fixed Cycles: Tapping / Thread Milling
4.4 T
A
PPING WITH CHIP BREAK
ING (Cy
c
le 209, DIN/ISO: G209)
Cycle parameters
U Setup clearance Q200 (incremental): Distance
between tool tip (at starting position) and workpiece
surface. Input range 0 to 99999.9999
U Thread depth Q201 (incremental): Distance
between workpiece surface and end of thread.
Input range –99999.9999 to 99999.9999
U 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
U Workpiece surface coordinate Q203 (absolute):
Coordinate of the workpiece surface. Input range:
-99999.9999 to 99999.9999
U 2nd setup clearance Q204 (incremental): Coordinate
in the spindle axis at which no collision between tool
and workpiece (fixtures) can occur. Input range 0 to
99999.9999
U Infeed depth for chip breaking Q257 (incremental):
Depth at which TNC carries out chip breaking. Input
range 0 to 99999.9999
U Retraction rate for chip breaking Q256: The TNC
multiplies the pitch Q239 by the programmed value
and retracts the tool by the calculated value during
chip breaking. If you enter Q256 = 0, the TNC retracts
the tool completely from the hole (to the setup
clearance) for chip breaking. Input range 0.1000 to
99999.9999
U Angle for spindle orientation Q336 (absolute): Angle
at which the TNC positions the tool before machining
the thread. This allows you to regroove the thread, if
required. Input range –360.0000 to 360.0000.
U RPM factor for retraction Q403: Factor by which the
TNC increases the spindle speed—and therefore also
the retraction feed rate—when retracting from the
drill hole. Input range 0.0001 to 10, rpm is increased
at most to the maximum speed of the active gear
range.
Retracting after a program interruption
If you interrupt program run during thread cutting with the machine
stop button, the TNC will display the MANUAL OPERATION soft key.
If you press the MANUAL OPERATION key, you can retract the tool
under program control. Simply press the positive axis direction button
of the active spindle axis.
Example: NC blocks
26 CYCL DEF 209 TAPPING W/ CHIP BRKG
Q200=2 ;SETUP CLEARANCE
Q201=-20 ;DEPTH
Q239=+1 ;PITCH
Q203=+25 ;SURFACE COORDINATE
Q204=50 ;2ND SETUP CLEARANCE
Q257=5 ;DEPTH FOR CHIP BRKNG
Q256=+25 ;DIST. FOR CHIP BRKNG
Q336=50 ;ANGLE OF SPINDLE
Q403=1.5 ;RPM FACTOR
Z
X
Q203
Q204
Q200
Q201
Q239