Internal Thread Processing: How Threads Are Cut Inside a Hole

• 1
  What actually happens at the cutting edge
• 2
  Cutting, forming and milling compared
• 3
  Class of fit, depth and inspection
• 4
  Where internal thread processing goes wrong
• 5
  Which internal thread processing method fits

An internal thread is a helical groove cut or formed on the wall of a drilled or bored hole. The tool has to enter a confined space, so chip evacuation and tool stiffness decide the result more than the nominal thread size does. A 60° thread form per ISO 68-1 or a 60° UN form per ASME B1.1 gives the same basic geometry; the flank angle and pitch control how load spreads across the engaged turns.

Cutting taps remove material. The tap flute carries chips backward out of the hole or forward through it. Forming taps do the opposite: they cold-form the wall, displacing metal into the crest and root instead of cutting it. That leaves an unbroken grain flow, which raises fatigue strength in the thread root, but it also needs a larger pre-drill hole because the material has to go somewhere.

The pre-drill diameter matters in both cases. For a cutting tap the rule is nominal diameter minus pitch: M8 × 1.25 needs a 6.75 mm hole, and a 1/4-20 UNC needs a 5.35 mm hole. For a forming tap you subtract roughly half the pitch, so M8 × 1.25 wants about 7.4 mm. Drill too small with a forming tap and the tap breaks. Drill too large and the thread is incomplete at the crest.

Engagement length is the other number that gets ignored. A thread needs enough engaged turns to carry the load. In steel, a common rule is one times the nominal diameter of full thread for a through hole; in aluminium it moves toward 1.5×. Below that, the thread strips before the bolt does, which is the failure nobody wants.

• 1
  Cutting tapRemoves material, works in almost any material
• 2
  Forming tapDisplaces material, no chips, stronger root
• 3
  Thread millSingle-point helix, one tool for many sizes
• 4
  Engagement1× nominal diameter in steel is a starting rule

Tapping is the default because it is fast. A cutting tap runs at 15–30 m/min surface speed in 1045 steel and 60–120 m/min in 6061 aluminium, with a feed locked to the pitch. The weakness is the chip. In a blind hole you need a spiral-flute tap that pushes chips back out of the hole, or a spiral-point tap that pushes them forward when there is room below. Get that wrong and the tap jams and snaps, usually on the second or third hole.

Thread milling uses a single-point or multi-tooth cutter that orbits the bore while the machine interpolates a helix. One tool covers a range of diameters and pitches, and it cuts interrupted threads, oversized threads and threads in hard material that would break a tap. The trade is cycle time. A thread mill typically runs 3–8 times longer per hole than a tap, and it needs a machine that can hold the helical interpolation without rounding the lead.

Forming taps run at higher surface speed than cutting taps in the same material and produce no chips at all. That is a real advantage in medical and food-equipment parts where a trapped chip is a contamination risk. The limits are material ductility and hole size. In 6061 or 304 stainless, forming works well. In cast iron, grey or ductile, the material has almost no elongation and the tap will crack the wall instead of forming it.

Single-point boring with a threading insert is the slowest option and the most controllable. It suits large bores above roughly 25 mm, unusual pitches, and parts where the thread must be corrected after heat treatment. The tool touches one flank at a time, so cutting forces stay low and the thread can be measured and adjusted on the machine.

• 1
  TappingFastest, needs correct flute geometry for the hole
• 2
  FormingNo chips, better root, needs ductile material
• 3
  Thread millingFlexible, slower, handles hard material
• 4
  Single-pointLarge bores and custom pitches, low force

Thread tolerance classes set how much play sits between the internal and external thread. A 6H internal thread is the general-purpose metric class and pairs with a 6g bolt. A 6G is looser and easier to assemble after plating, which matters because electroless nickel or anodizing adds thickness on the flanks. On inch threads, 2B is the normal internal class and 3B is the tight one used where vibration loosening is a concern.

Plating is the trap. A 6H thread that is anodized or nickel-plated can close up enough that a 6g bolt will not enter without force. The usual fix is to specify a 6G or a pre-plate allowance, or to mask the thread. State it on the drawing; a shop cannot guess which threads will be coated later.

Depth is measured from the start of the thread to the last full thread, not to the drill point. A blind hole needs a drill depth about one diameter deeper than the thread depth to leave room for the tap lead. A thread that is 10 mm deep in an M6 hole needs a drilled depth near 16 mm. If the drawing calls out 10 mm of full thread and the hole is 11 mm deep, the tap will bottom out before the thread is complete.

Inspection uses go/no-go gauges for production and thread wires or a thread micrometer for setup. Optical comparators and CMM thread scanning are used when the flank angle or pitch diameter on a critical part has to be documented. We run a go/no-go check on every threaded feature before the part leaves the machine, and we record it on the inspection report.

• 1
  6H / 2BGeneral-purpose class for most metal parts
• 2
  6G / 3BLooser or tighter depending on assembly need
• 3
  PlatingAdd a pre-plate allowance or mask the thread
• 4
  Drill depthAbout one diameter beyond the thread depth

Thin walls are the most common failure. When the wall around a tapped hole is thinner than about half the thread diameter, the wall bulges outward as the tap forms or cuts, and the thread comes out out-of-round. Reducing the hole size does not help. The better answer is to add a boss, switch to thread milling so the cutting force drops, or move the hole to a thicker section.

Hard material changes the method. Above roughly 35 HRC, a cutting tap wears fast and the torque climbs until something breaks. Thread milling with a carbide cutter handles 45–55 HRC without much trouble, and it lets you cut the thread after heat treatment instead of before. If the part is hardened after threading, plan on a cleanup pass, because distortion will move the pitch diameter.

Deep holes and long tools run into deflection. A tap with a length-to-diameter ratio above 4:1 will wander, and the thread will not be square to the face. Use a spiral-flute tap with a reduced shank, peck the cycle, or move to thread milling where the tool is stiffer per unit of reach. On bores deeper than 5× the diameter, single-point boring is often the only method that holds the lead straight.

Material choice sets the speed. Aluminium 6061 and 7075 tap fast and form well. Stainless 304 work-hardens at the surface if the tool rubs, so keep the feed per tooth up and never dwell. Titanium Ti-6Al-4V needs slow speed, plenty of coolant and sharp tools; a dull tap will gall and seize in the hole. Inconel and other nickel alloys are usually thread-milled rather than tapped.

• 1
  Thin wallBelow half the thread diameter, expect ovality
• 2
  Hard steelAbove 35 HRC, thread mill instead of tap
• 3
  Deep holeOver 4:1 length to diameter, use thread milling
• 4
  StainlessKeep feed up, do not let the tool rub