CNC Fanuc G76 Threading Cycle

Threading is an integral part of almost every component which is machined, threads may be internal (ID threading) or external (OD threading). Here is full explanation of G76 Threading Canned Cycle for the Fanuc cnc control.

The CNC G-code for the threading canned cycle is G76.

You might like other cnc threading cycle G92, G32, G33,

Below 2 block Fanuc G76 threading cycle ( Two Line Format G76 Threading Cycle) is briefly explained for easy understanding of g76 threading code.

Contents

Fanuc G76 Threading Cycle can be used for

Fanuc G76 Threading Cycle Flexibility

With Fanuc G76 Threading Cycle you can control

Number of Spring Cuts or Spring Passes on fanuc G76 thread cycle.
Infeed Angle
Depth of Normal Cuts
Depth of Finish Cut
Depth of First Cut

and many more.

G76 Threading Cycle Example

Example of the G76 G code G76 Thread Cycle a CNC Programming Example.

Fanuc G76 Threading Cycle Explanation

N5 G76 P010060 Q100 R0.05

N6 G76 X30 Z-20 P1024 Q200 F2

First block of the G76 Threading cycle

G76 : G code for threading cycle.

P : P actually consists of multiple values which control the thread behavior,

01 : Number of spring passes or spring cuts.
00 : Thread run out at 45 degree
60 : Flank angle or In feed angle

Q : Depth of normal cut ( these values are given in hundreds, so the depth of cut will be 0.1 ).
R : Depth of Last or Finish cut

Second block of the G76 Threading cycle

G76 : G code of the threading cycle.
X : The end value in x-axis.
Z : The end value in z-axis.
P : Thread depth ( as radius value ).
Q : Depth of first cut.
F : Thread Pitch
R : Thread Taper

Tapered Threading with Fanuc G76 Threading Cycle

Taper threading is not a usual practice in cnc machine workshops, but sometimes customer want a component with taper threading, So here is the solution. Taper threading on a cnc lathe machine with Fanuc control is just easy with Fanuc G76 threading cycle. Fanuc CNC control threading cycle G76 gives us lot of flexibility.CNC Programming tapered threading with Fanuc threading cycle G76 is not that difficult, just one parameter have to add.

Contents

How to calculate R parameter for Tapered Threading on Fanuc with G76 Threading Cycle.

Normal Threading with Fanuc G76 Threading Cycle CNC Program

N5 G76 P010060 Q100 R0.05

N6 G76 X30 Z-20 P1024 Q200 F2

One G76 parameter which have to be added for tapered threading is R in G76 second block.

Tapered Threading with Fanuc G76 Threading Cycle CNC Program

Tapered Threading with Fanuc G76 Threading Cycle

N5 G00 X50 Z5

N6 G76 P010060 Q100 R0.05

N7 G76 X43 Z-45 P1024 Q200 R-14.5 F2

Other parameter of Fanuc threading cycle G76 are explained here.

The R parameter in second block of G76 is the tapered value. Note that R is given as Radius value.

How to calculate R parameter for Tapered Threading on Fanuc with G76 Threading Cycle.

R = (Start Diameter – End Diameter) / 2

Controlling Threading Infeed Angle with Fanuc G76 Threading Cycle

Briefly described how to control thread infeed angle while machining threading on a cnc machine with fanuc cnc control.

You better watch the video ( Thread Infeed Tips from Sandvik Coromant a Video ) which briefly describes the difference of thread infeed angles and benefits and weaknesses of different thread infeed angles.

Fanuc G76 threading cycle gives us full flexibility to thread the way we like.

Contents

Fanuc G76 Threading Cycle

Fanuc G76 Threading Cycle

N5 G76 P010060 Q100 R0.05

N6 G76 X30 Z-20 P1024 Q200 F2

Controlling Thread Infeed Angle with Fanuc Threading Cycle G76

G76 : Threading Cycle Parameter P P actually consists of multiple values which control the thread behavior,

01 : Number of spring cuts, you can change it at your will.
00 : Thread run out at 45 degree
60 : Thread Infeed Angle / Flank angle

All the parameters of Fanuc threading cycle G76 are fully explained here. The values with P are actually 03 pairs of values, the last pair is to control the thread infeed angle of each pass for threading, You can see the bold line above with value 60.

G76 Threading Cycle with 60 Degrees Infeed Angle for 60 Degree Threads (Compound Infeed/ Flank Infeed)

If you put 60 for the infeed angle, this will put most of the load on the front edge of the threading insert.

G76 Threading Cycle with 55 Degrees Infeed Angle for 60 Degree Threads

If you put 55 for the infeed angle for the standard 60 degree threads, this will put most of the load on the front edge or leading edge of the threading insert and will also put a small load on the back edge of the threading insert.

G76 Threading Cycle with 0 Degrees Infeed Angle ( Radial Infeed)

If you put 0 for the infeed angle, this will put the load on the full profile of the threading insert.

Square thread always need a straight radial infeed (plunge infeed ).

G76 Threading Cycle Recommended Infeed Angles

The following indeef angles should be used as infeed angles with G76 fanuc threading cycle. 80, 60, 55, 30, 29, 00

G76 Thread Cycle a CNC Programming Example

G-code G76 is a cnc cycle which is used for thread cutting on cnc machines.
Threading cycle G76 is explained here G76 Thread Cycle.
Taper thread cutting with G76 thread cycle is explained here G76 Tapered Threading
For Multi-start thread cutting with G76 see G76 Multi-Start Threading
For G76 threading cycle one line see G76 One-Line Format.
G76 threading cycle can be used for internal threading on cnc lathe machines.
This G76 threading example actually cuts external threads on two different diameters.

G76 Thread Cycle Example

G76 Thread Cycle a CNC Programming Example

N10 T3

N20 G97 S800 M03

N30 G00 X30 Z5 T0303

N40 G76 P021060 QI00 R100

N50 G76 X18.2 Z-20 P900 Q200 FI.5

N60 G00 X50 Z-20

N70 G76 P021060 Ql00 R100

N80 G76 X38.2 Z-52 P900 Q200 FI .5

N90 G00 X200 Z200

N100 M30

cara memprogram cnc dasar

Rabu, 17 Agustus 2016