As a robot, how much do you know about the thread code comparison table?

A thread code is read left to right. The letters are the family and the standard behind it. BSW is British Standard Whitworth, coarse series, 55° thread angle. BSF is the same form in a fine series. UN is the Unified National form used in the US, 60° angle, and it splits into UNC, UNF and UNEF. M means metric, ISO 68-1 form, 60° angle. G is a non-sealed parallel pipe thread, also called BSPP. R and Rc are tapered pipe threads, R external and Rc internal.

The trap is that two families share a nominal size and share nothing else. A 1/2 in bolt is not a 1/2 in pipe. UNC 1/2-13 is 12.7 mm major diameter with 13 threads per inch. G 1/2 pipe has an outside diameter of about 20.96 mm. If a drawing says 1/2 and nothing else, it is not a thread specification yet.

Old codes still circulate. Zg and Kg are older designations for tapered pipe threads and map to R and Rc. When a legacy drawing lands on the shop floor we convert the callout to the current standard and confirm with the customer before cutting. That confirmation costs an email. Recutting a 316L manifold costs a lot more.

• 1
  Letters firstBSW, BSF, UN, M, G, R and Rc are different families, not synonyms.
• 2
  Pitch is separateCoarse or fine is a second decision after the family.
• 3
  Pipe is not boltPipe sizes are nominal bore, not outside diameter.

Metric callouts read diameter then pitch: M8 × 1.25 is 8 mm major diameter with a 1.25 mm pitch. Drop the pitch and you get the coarse default, M8 × 1.25. Inch callouts read diameter in inches then threads per inch: 1/4-20 UNC is 0.25 in diameter with 20 threads per inch. Both systems let you write a fine pitch that also exists as a UNF or a metric fine. Write the pitch out. It removes the guess.

Class is where most drawings go quiet. Unified classes run 1B, 2B and 3B for internal threads, and 1A, 2A and 3A for external. Class 2 is the normal commercial fit. Class 3 is a tighter controlled fit for high-strength or precision assemblies. Metric uses 6H for internal and 6g for external as the default, with 4H, 5H, 4g and 5g for tighter work. A 1/4-20 UNC 2B hole and a 1/4-20 UNC 3B hole take different tap drill sizes and different inspection gauges.

Then check whether the thread is a fit or a seal. Straight G threads do not seal on the flank. They seal on a bonded washer or an O-ring face. Tapered R, Rc and NPT threads seal by deformation of the flanks as they tighten. That is why a G 1/2 port machined with an R 1/2 tap will thread in and still leak under pressure.

Thread milling wins on hard material and on large diameters. A single-point or multi-flute mill cuts Inconel and 17-4PH without the torque spike of a tap, and one tool covers a range of diameters by changing the helical path. Chip evacuation is easier in a blind hole. The trade is cycle time, which matters more below about M6.

Tapping is faster and cheaper on small holes in aluminium, brass and mild steel. It becomes risky in titanium and in any hole deeper than two times the diameter, where chip packing breaks taps. Roll forming is the third option. It cold-forms the thread instead of cutting it, gives a stronger root, and produces no chips, which is useful on medical parts where a trapped chip is a reject. Roll forming needs a specific hole diameter and works best in ductile material under 32 HRC.

For pipe threads we prefer single-point on a lathe or mill-turn center. A 4,000 mm maximum processing size and a Ø400 mm rotary table let us hold a long manifold and cut a tapered port in the same setup as the sealing face. Cutting the port and the face together is how you keep the thread concentric to the seat. Separate setups stack two tolerances.

• 1
  Thread millHard alloys, large sizes, blind holes, one tool per family.
• 2
  TapSmall holes, soft material, through holes, high volume.
• 3
  Roll formChip-free threads, stronger root, ductile material below 32 HRC.

A thread is a form, so it is checked with go and no-go gauges, not with calipers. The go gauge must enter by hand for the full length. The no-go gauge should not enter more than two or three turns. For critical parts we add a pitch diameter measurement and a thread profile check on an optical comparator. Plug gauges cover internal threads, ring gauges cover external ones.

Pipe threads add a step. The gauge has a notch or a step on the end face, and the acceptance is how far the thread sits relative to that face. A 1/2 NPT port that passes go and no-go can still be too shallow or too deep for the mating fitting. We check that face position on every pipe port, because it is the dimension that decides whether the joint seals.

Material changes the plan. Threads in 6061-T6 aluminium and 303 stainless cut clean and gauge predictably. 316L work-hardens and needs sharper tools and lighter passes. Titanium TC4 (Ti-6Al-4V) galls, so we run slower speeds and check the gauge more often. On a 10,000+ part run we inspect at the machine and again at final, with reports available on request.