Word meanings in the G76 threading command

As you know, turning centers that have Fanuc and Fanuc-compatible controls have a multiple repetitive cycle (G76) that dramatically simplifies the programming of threading operations. While it is a usually a very simple command to use, there are some tricks to using it – especially with more complex threads.

Prior to the G76 command in a program, the spindle must be started. Most machine tool builders recommend that threading be done in the lowest spindle range (if the machine has more than one) and in RPM mode (constant surface speed mode will cause undesirable spindle speed changes for each pass).

The threading tool must then be sent to a convenient starting position. For external threads, this will be to a diameter that is larger than the major diameter of the thread. For internal threads, this will be a diameter that is smaller than the minor diameter of the thread. In Z, the convenient starting position should be about four times the thread pitch or 0.2 in, whichever is smaller. This approach distance in Z will ensure that the Z axis is moving at the desired feedrate (fully accelerated) prior to machining.

Note that Fanuc actually has two different ways to command G76, based upon control model. With most, a one-line G76 command is given.

Basic words for straight threads and what they do:

  • G76 – this commands the threading operation

  • X – for external threads, this will be the minor diameter of the thread. For internal threads, it will be the thread’s major diameter

  • Z – this is the end point of the thread in Z – the tool will move from the convenient starting position (or close to it) to this location during each pass.

  • K – this is the depth of the thread – the distance (on the side) from the major diameter of the thread to the minor diameter

  • D – this is the depth of the first pass. For external thread, the X position for the first pass can be calculated by adding twice the G76 K value to the G76 X value and subtracting twice the G76 D value. Subsequent passes will be shallower. And the number of passes can be difficult to calculate (formula to calculate number of passes is given in the Fanuc manual – good luck). Generally, if you want more passes, reduce the value of D. To make fewer passes, increase the value of D.

  • A – this is the included angle of the thread form. For National Standard threads, it will be 60 degrees (A60). Other thread forms require a different A word. Note that most controls limit the number of different A word values available. You must reference your programming manual to find them. When A is (correctly) specified, the threading tool will machine only on its front edge, which is required for traditional threading tools. There are, however, threading tool manufacturers that require their threading tools to be plunged straight in (forcing the tool to cut on both sides of the insert). To accomplish this, A can be left out of the G76 command, or it can be included and set to zero (A0).

  • F – this is the feedrate in inches per revolution, which will be equal to the thread’s pitch. For threads dimensioned in the Imperial (inch) measurement system, pitch is calculated by dividing one by the number of threads per inch.

Taper threading

To machine taper threads, an I word is included in the G76 command. I is the distance and direction along the X axis (a radial value) from the end point of the thread to the start point of the thread. For external threads, I will be negative. For internal threads, I will be positive. To calculate this distance, multiply the full Z axis travel distance for each pass (including approach) times the tangent of the taper angle.

Multiple start threads

One way to machine multiple start threads is to specify one G76 command per thread start. Between starts, move the tool over in Z by a distance of one divided by the number of starts times the lead. For a 0.5 lead thread with four starts, the tool will be moved over 0.125 between passes.

Some controls provide another word for the G76 command that specifies the entry angle for the thread start. This eliminates the need to move the tool between passes. For these controls, the letter address Q is used. For a four start thread, the Q word will be Q0 in the first G76 command, Q90. in the second, Q180. in the third, and Q270. in the last.

50 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

cnc reverse logo.jpg

44 Little Cahill Road

Cary, IL  60013

Ph: 847-639-8847

  • Facebook Social Icon