G76 Cycles – Thread Turning Gcode Programming

It’s essential to have a solid understanding of the terms that define the Gcode thread cycles before starting to program it!

Infeed methods

There are several methods to program how the threading tool enters the material, each with its own advantages and disadvantages, making each one suitable for different scenarios. 

Radial Infeed

It is the most straightforward method available on all controllers and can also be used on a manual lathe.

Common use cases:

• Fine pitches below 16 TPI (1.5 mm).
• Short-chipping materials such as brass and free-cutting steel.

Flank Feed

A good all-around choice that is available on all controllers.

Common use cases:

• Coarse pitches above 24 TPI (1 mm).
• Trapez profiles (Acme threads)

Modified Flank

The method is the same as the flank feed method, but it is slightly angled to avoid the insert edge rubbing against the component surface. It is not supported by all controllers. However, if your controller supports it, it is a better choice than the “regular” flank method.

The implementation is by subtracting twice the slant angle from the profile angle. For example, for a 60° thread with a modified flank cycle with 3°, you should enter 60-2X3=56° instead of 60°

Alternating Flank

In this method, the cutting tool engages with the workpiece on each pass from the opposite side, resulting in an even distribution of wear. Not supported by all controllers.

Common use case: Longer tool-life becomes more beneficial in pitches greater than 5 TPI (5 mm) with much material to remove.

Depth per Pass

The lead determines the feedrate and is much larger than regular feeds used in turning operations. The profile height dictates the total depth of the cut. Therefore, cutting the thread in multiple passes is the only way to control the chip load. There are two methods to divide the total depth into multiple passes.

Constant Depth

The depth is divided equally between the passes. The depth of cut is the same in each pass; hence, the chipload increases from pass to pass.

\( ap_n=\large \frac {\text{Profile Height} – \text{Finish Pass}}{\text{Number of Passes}} \)

Constant Volume

The depth is decreased in each pass to maintain a consistent chip load.

\( n = \text {Pass number} \)
\( ap_1 = \large \frac {\text{Profile Height} – \text{Finish Pass}} {\sqrt{\text {Number of Passes}}} \)
\( ap_n = ap_1 \times \left [\sqrt{n} – \sqrt {\left ( n -1 \right )} \right ] \)

Determining the thread height (Porife depth)

The profile depth (thread height) you need for programming a thread cycle is

External thread:

From the flat (or rounded) crest, which is the major diameter to the theoretical apex of the root. In 60 degrees parallel threads like standard metric and inch threads, it equals 0.61343 * Pitch

Internal thread:

From the flat (or rounded) crest, which is the minor diameter to the theoretical apex of the root. In 60 degrees parallel threads like standard metric and inch threads, it equals 0.57364 * Pitch

Determining the first cut depth

The threading cycles calculate internally the required number of passes and the depth of each to maintain a constant volume or depth, according to the depth of the first pass. There are two approaches to deciding its value. (The number of passes is not a parameter entered into any of the threading cycles!)

Option 1:

Decide what is the largest depth you think your cutting edge can take. The controller will decide on the number of passes to maintain the same chip load as in the first pass (The depth in each pass will be reduced). In this method, no calculations are needed.

Option 2:

Decide how many passes you want and calculate the depth of the first pass according to the below formulas:

Additional parameters

Some controllers provide additional parameters to customize the cycle.

• Add a chamfer at the end of the thread (Not supported by all the controllers)
• Add an additional finish pass after the constant depth/volume passes sequence. (Not supported by all the controllers)

* Learn more about Single-point thread programming

Which options are supported by your controller?

* Options that don’t appear on the above chart are available on all the controllers.

Now that we know how to determine the parameters, it is time to see the Gcode syntax for the common threading cycles

Fanuc G76 threading cycle (two lines format)

This format is applicable for: 

• Fanuc types A, B, and C. (On C type, replace G76 with G78)
• Mazak
• Mitsubishi

Line 1: 

P = A six-digit code in three pairs:

Digits 1 and 2 – number of finishing cuts (01-99). Usually 00 or 01.

Digits 3 and 4 – Chamfer size expressed as a percentage of the lead. 00 means without a chamfer.

Digits 5 and 6 – Thread V angle (00, 29, 30, 55, 60, 80 degrees only). 00 is used for radial infeed.

Q = The minimum allowed cutting depth expressed in microns. If, according to the calculations, smaller depths are needed, they will be ignored. This parameter is used to restrict unnecessary passes with ridiculously small depths.

R = The depth of the additional finish pass. (0.0 if none)

Line 2:

X = The diameter of the last pass. (Minor diameter in external threads / and major diameter in internal threads). You should use the diameters as explained here and not the major/minor diameters used for measurements!

Z = The thread’s end along the axial axis.

R = The amount of taper over the total length (per side). Used for NPT & BSPT threads. Enter 0.0 for parallel threads.

P = Profile height (see above), expressed in microns.

Q = The depth of the first threading pass (see above), expressed in microns.

 F = the feed rate, which equals the thread’s lead (Or the pitch in single-start threads).

In Mazak and Mitsubishi controllers:

* There is an additional P parameter at the end of line 2 (after the F) that determines the in-feed method:

P1 = Constant Volume.

P3 = Constant depth.

* All the parameres are expressed in mm/inches (Not in microns)

To see Gocde examples with the different options, change them in the GCODE GENERATOR above and check how they reflect in the program!

Fanuc G76 threading cycle (one-line format)

This format is applicable for: 

• Fanuc T series (T6, T11, T15, etc.)
• Haas

X = The diameter of the last pass. (Minor diameter in external threads / and major diameter in internal threads). You should use the diameters as explained here and not the major/minor diameters used for measurements!

Z = The thread’s end along the axial axis.

I = the amount of taper over the total length (per side). Used for NPT & BSPT threads. Enter 0 for parallel threads.

K = Profile height (see above), expressed in microns.

D = The depth of the first threading pass (see above), expressed in microns.

A = Thread V angle (00, 29, 30, 55, 60, 80 degrees only). 00 is used for radial infeed.

F = The feed rate, which equals the thread’s lead (Or the pitch in single-start threads).

P – Infeed method adjustment:

P1 = Flank/modified flank feed with constant volume

P2 = Alternating flank feed with constant volume.

P3 = Flank/modified flank feed with constant depth

P4 = Alternating flank feed with constant depth.

Q = Spindle rotation shift angle. The data range is from 0 to +/-360000 (360 degrees = 360000, without decimal point) This function is used for cutting multiple-lead threads. In the case of a 3-start thread, the shift angle between each thread is 120 degrees. This means that to cut the first thread lead, we use Q=0. To cut the second and third thread leads, we use Q=120000 and Q=240000, respectively. It’s important to note that the Z-axis start position remains the same for each thread.

Additional parameters for Haas controllers

M – Chamfering.

M23 = With chamfer

M24 = Without chamfer

* On Haas controllers, all the values are entered in mm/Icnhes (Not in microns!)

To see Gocde examples with the different options, change them in the GCODE GENERATOR above and check how they reflect in the program!

Okuma G71 threading cycle

Okuma controllers utilize a different cycle (G71), which includes all the aforementioned options and additional ones. This is the most comprehensive thread cycle available.

X = The diameter of the last pass. (Minor diameter in external threads / and major diameter in internal threads). You should use the diameters as explained here and not the major/minor diameters used for measurements!

Z = The thread’s end along the axial axis.

A = Taper angle. (For BSP/NPT threads)

I = Difference in radius between the starting point and end point (expressed as a radius).

* You can use either an A or I mode (Not both).

B = Thread V angle (e.g., 60, 55, 29)

D = The depth of the first threading pass (see above), expressed as a diameter.

U = The depth of the additional finish pass (0.0 if none), expressed as a diameter.

H = Profile height (see above), expressed as a diameter.

L = Chamfering distance in final thread cutting cycle(Effective in M23 mode; if no L word is designated in the M23 mode, L is assumed to be the distance equivalent to one lead.)

E = Lead variation rate per lead for variable lead thread

F = The feed rate, which equals the thread’s lead (Or the pitch in single-start threads).

J = Number of threads within a distance specified by F word (When no J word is designated, the control assumes J=1)

Q = Number of threads for multi-thread thread cutting.

M – Thread cutting pattern and mode of infeed. (Up to 3 M-codes are allowed – One from each set)

Set 1

M74 =Constant Depth

M75 =Constant Volume

Set 2

M32 = Flank Infeed (Right flank)

M33 = Alternating Flank Infeed

M34 = Flank Infeed (Left flank)

Set 3

M22 = No Chamfer

M23 = With Chamfer

To see Gocde examples with the different options, change them in the GCODE GENERATOR above and check how they reflect in the program!