Haas G76 threading cycle can be used for, external threads, Internal threads, straight threads, taper threads.
With Haas G76 threading cycle, a programmer can easily command multiple cutting passes along the length of the thread.
The nature of tool load and wear can be controlled by using the P code. The P code can specify which side the tool
cuts on and it can specify how much material will be cut.
Haas G76 Threading Cycle Applications
Hass G76 thread cutting cycle can be used for,
- Internal threading (I.D. thread cutting).
- External threading (O.D. thread cutting).
- Straight threading.
- Taper threading.
Haas G76 Threading Cycle Format
G76 X(U) Z(W) K D A F(E) I P Q
X – X-axis absolute location, maximum thread Depth Diameter (optional).
Z – Z-axis absolute location, maximum thread length (optional).
K – Thread height, defines thread depth, radius measure.
D – First pass cutting depth.
A – Tool nose angle (value: 0 to 120 degrees).
F(E) – Feed rate, the lead of the thread.
U – X-axis incremental distance, start to maximum thread Depth Diameter (optional).
W – Z-axis incremental distance, start to maximum thread length (optional).
I – Thread taper amount, radius measure (optional).
P – Single Edge Cutting (load constant) (optional).
Q – Thread Start Angle (Do not use a decimal point) (optional).
Setting 95 – Thread Chamfer Size.
Setting 96 – Thread Chamfer Angle.
Setting 86 – Thread Finish Allowance.
M23 – Chamfering ON
M24 – Chamfering OFF
Haas G76 Threading Cycle Parameter Explanations
K -Thread height
The height of the thread is defined as the distance from the crest of thread to the root of the thread.
The calculated depth of thread (K) will be the value of K less the finish allowance (Setting 86, Thread Finish Allowance) is this amount.
D – First pass cutting depth
The depth of the first cut through the thread is specified in D. The depth of the last cut through the thread can be controlled with Setting 86.
At the end of the thread an optional chamfer is performed.
The size and angle of the chamfer is controlled with Setting 95 (Thread Chamfer Size) and Setting 96 (Thread Chamfer Angle).
P – Single Edge Cutting (load constant) (optional)
Four options for G76 Multiple Thread Cutting are available
- P1:Single edge cutting, cutting amount constant
- P2:Double edge cutting, cutting amount constant
- P3: Single edge cutting, cutting depth constant
- P4: Double edge cutting, cutting depth constant