top of page

Some special feature of G76 (the threading command)

Fanuc's threading command is pretty powerful - and very helpful. It will allow you to completely machine a thread with one command in your program, regardless of how many passes the threading tool must make. The G76 command is given after the threading tool approaches the diameter to be threaded - away from the diameter in Z and above or below the diameter in X (above for outside diameter threads and below for inside diameter threads).

Though the actual words given for G76 will vary even among Fanuc controls, the functions they control include:

  • Major/minor diameter of the thread (major for ID threads and minor for OD threads) - This is done with the X word for all Fanuc control models.

  • End point for threading - This is done with the Z word.

  • Total thread depth - This is a radial value (again, actual thread depth) and is done with either the K word or P word depending upon control model.

  • Depth of first pass - This controls how many passes will be made. The machine will make shallower and shallower successive passes. The word that controls this could be a D word or Q word, depending on model.

  • Thread pitch - Done with the F word with all control models, this controls the feedrate for threading.

  • Tool angle - This specifies how the thread will be machined. If this value is specified, the control will machine on only the front side of the threading insert (as is normally desired). If this value is not specified, the tool will machine on both sides of the insert (plunging straight in). An A or P word specifies tool angle, depending upon model.

Again, the functions just described are pretty basic, and consistent from one thread to another. Here is an example command that machines an OD thread (approach position is above X value in threading command).:

  • O0016 (Program number)

  • N005 T0505 M41 (Select external threading tool and low spindle range)

  • N010 G97 S500 M03 (Start spindle fwd at 500 rpm)

  • N015 G00 X5.7 Z-0.8 M08 (Rapid to convenient starting position, start coolant)

  • N020 G76 X5.392 Z-1.88 K0.054 D0100 A60 F0.0625 (Chase 5.5-16 thread)

  • N025 G00 X8.0 Z6.0 (Rapid to safe index position)

  • N030 M01 (Optional stop)

  • .

  • .

  • .

If you have been using the G76 command on a regular basis, so far we haven't told you anything new. But there are some special, lesser-known functions of G76 that we'd like to relate.

Taper threading

When machining a taper thread, of course, the tool must make a tapered move when threading. The amount of taper is specified with an I word or R word, depending upon control model. This word does not specify the taper angle. Instead, it specifies the distance and direction from the end point of the thread to the start point of the thread along the X axis. For OD threads, this value will be negative - for ID threads, it will be positive (assuming you are machining in the negative Z direction, as is normally the case).

To calculate the value of this word, you must know the taper angle, which is 3.718 degrees for National Standard threads. You multiply the tangent of the taper angle times the total distance in Z that the tool will be moving during each pass (including approach).

Multiple start threads

Some controls require that you specifies more than one G76 command when machining a multiples start thread (one for each thread start. This requires a Z axis movement between threading commands. The amount of movement is the pitch of the thread (total lead divided by the number or thread starts). For a four-start thread with a 0.5 inch overall lead, the pitch is 0.125.

In some cases, it may not be possible to move in Z between passes (consider a thread at the end of the workpiece that is supported by a tailstock). And the extra motion does take time, making for a somewhat inefficient cycle.

Newer controls have overcome these two limitations. A Q word in each G76 command specifies the angle of entry for the treading tool. For a four-start thread, an example set of Q words is Q0, Q90.0, Q180.0, and Q270.0.

Not always programmable

There are some thread functions you should know about that may not be programmable. They are only programmable for control models that use a two-line G76 command (many 0T controls use this method). For controls that use the one-line G76 command, a parameter controls the function. If you want to change its value, you must change a control parameter.

Number of spring passes - This function, which is controlled by a P word for those controls that allow it to be programmed, controls what happens after the thread has been machined to its final depth. If left out, or if the value is zero, the machine will simple stop threading, ending the cycle. But if this value is set to something greater than zero, the control will continue, with each successive pass being of zero depth. These passes, which are commonly referred to as spring passes, allow tool pressure to be relieved.

Chamfer amount - This function, which is controlled by a P word for those controls that allow it to be programmed, controls how the tool pulls away from the thread at the end of each pass. If set to zero (or left out of the command), the tool will move to the value specified by the Z word (end point of the thread) and pull straight away in the X axis. If this value is greater than zero, the tool will come to within this value of the thread's Z end point and begin angling out at a 45 degree angle. For most threads - especially those with a thread relief groove, it is best to leave this value at zero.

Minimum depth of cut - As stated, the machine will proceed to make shallower and shallower passes. This value provides a cutoff point, from which passes do not get any deeper. This function is controlled by a Q word for those controls that allow it to be programmed.

Final pass depth - This value is specified by an R word for those controls that allow it to be programmed.

1,776 views0 comments

Recent Posts

See All

Tapping on a turning center (without canned cycles)

Unless your Fanuc controlled turning center came with live tooling, it’s likely that you don’t have canned cycles (G80-G89) like those you find on machining centers. You might have G74 and G75, the mu

Can you speed up your tool change time?

Machining centers, of course, have automatic tool changing devices to automate the tool changing process. Current models boast very fast tool changing times and you may be quite satisfied with tool ch


bottom of page