Thread turning with G76

How it is calculated

The thread height and the root come from the basic profile of the ISO metric thread. With P the pitch,

For an external thread 0.6134 P is half the difference between the major diameter d and the root diameter d3 = d − 1.2269 P, so the root X is d − 2h. For an internal thread 0.5413 P is half of D − D1, so the thread runs from the bore D1 out to X = D. These are basic sizes, with no tolerance class. An external 6g thread is a little under the basic size, and the bore of a 6H internal thread is at D1 or a little over. Turn the outside a little under D before threading (for example Ø19.85 for M20×1.5), then set the final size with a thread ring gauge or plug gauge, or by measuring the pitch diameter, and correct X or the wear offset.

Unified inch threads (UNC, UNF) have the same 60° basic profile as ISO metric threads, so the same heights apply with the pitch P = 25.4 ÷ TPI. On a machine programmed in millimetres (G21) the lead F is written to four decimals, for example F1.9538 for 13 TPI. The error left by rounding is under 0.001 mm over a 30 mm thread, while three decimals (F1.954) leave about 0.002 mm. The sizes in the list are converted to mm; with "Other", enter the diameter in inches.

BSP parallel pipe threads (G, ISO 228-1), and BSW, use the 55° Whitworth form with a rounded crest and root. The external and internal threads have the same height, h = 0.6403 P, so the root of an external thread is D − 1.2807 P and the bore of an internal thread is the same diameter. The last two digits of P in the first block are 55. Tapered pipe threads (NPT, BSPT R and Rc) are not covered: they need the taper R in the second block and a gauge length.

G76 cuts every pass with the same chip area. The groove is a V, so the area grows with the square of the depth, and the total depth after pass n is

Q is the first pass depth. When a pass would add less than the minimum depth, the control adds the minimum instead. The rough passes stop at h − R, and the finish passes cut to the full height h; the first removes the allowance R and the others pass again at the same depth. If you set the number of rough passes instead, the first pass depth is$Q = (h - R)/\sqrt{N}$, and the table shows the real count, which is lower when the minimum depth acts.

The table follows the formula. The last rough pass and the finish pass can differ slightly between control models.

G76 feeds the tool in down the flank that faces the start point, as Fig. 4.2.7 of the Fanuc 0i-F lathe manual draws it, so only one edge cuts. Each pass therefore starts back toward the start point by $(h - D_n)\tan(a/2)$, where a is the tool angle in the last two digits of P; the Start Z column gives it, and the finish pass starts at the programmed start Z. With 00 the tool feeds straight in and both edges cut. The manual draws threads cut toward −Z only; for a thread cut toward +Z the table mirrors the rule.

Rules that the page checks:

• Use G97 and keep the same S for every pass. The Z axis moves at lead × S mm/min; check that this is within the machine's maximum feed for threading.
• Start Z at least two to three leads from the start of the thread, so the axis reaches speed before the tool reaches the work. The page assumes the thread starts at Z0.
• With no chamfering (00) the thread end Z must be in the undercut. With chamfering the full-depth thread ends that distance before the end Z. In the two-block G76 the middle digits of P switch chamfering on and set its length, so no M code is needed; M23 and M24 belong to the older one-block G76.
• P and Q are whole micrometres with no decimal point.