HEIDENHAIN TNC 320 - Cycle Parameters

Fixed Cycles: Tapping / Thread Milling
4.2 TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206)
4
96
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
Cycle parameters
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface Input range
0 to 99999.9999
Guide value: 4x pitch.
Q201 Depth of thread? (incremental): Distance
between workpiece surface and root of thread.
Input range -99999.9999 to 99999.9999
Q206 Feed rate for plunging?: Traversing speed of
the tool in mm/min during tapping. Input range 0 to
99999.999 alternatively FAUTO
Q211 Dwell time at the depth?: Enter a value
between 0 and 0.5 seconds to avoid wedging of the
tool during retraction. Input range 0 to 3600.0000
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
NC blocks
25 CYCL DEF 206 TAPPING NEW
Q200=2 ;SET-UP CLEARANCE
Q201=-20 ;DEPTH OF THREAD
Q206=150 ;FEED RATE FOR
PLNGNG
Q211=0.25 ;DWELL TIME AT DEPTH
Q203=+25 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP
CLEARANCE
The feed rate is calculated as follows: F = S x p
F:
Feed rate (mm/min)
S:
Spindle speed (rpm)
p:
Thread pitch (mm)
Retracting after a program interruption
If you interrupt program run during tapping with the machine stop
button, the TNC will display a soft key with which you can retract
the tool.