Threaded holes are where a cheap part turns expensive. The thread is usually the last feature cut, it carries the tightest fit callout on the drawing, and it is the one place a broken tool can scrap a finished part outright. Two methods dominate: tapping, which cuts or forms the thread in one pass with a tool shaped like the thread itself, and thread milling, which interpolates the thread with a smaller cutter that spirals down the hole. Most shops default to tapping because it is fast and the tooling costs a few dollars. That default is wrong more often than people admit — in deep holes, in stainless and titanium, and anywhere a scrapped part costs more than the tap that broke inside it. This article lays out the real trade-offs: hole depth, material, chip control, tool life, and what a broken tap actually costs.
How tapping and thread milling actually cut
Tapping drives a tool shaped exactly like the finished thread into a pre-drilled hole. A cut tap is, in effect, a hardened screw with cutting edges and flutes; it is driven down at the thread pitch, shears the material into chips that travel back up the flutes, and then reverses out to clear. One pass, one thread, done. That is the entire appeal, and it is a real one: the cycle is seconds, and a quality tap costs a few dollars.
A form tap, sometimes called a roll tap, does not cut at all. It cold-forms the thread by displacing material, so it produces no chips to evacuate and no cut grain to weaken the root. It needs a slightly larger pre-drill and only works in ductile material — aluminum, mild steel, some brass — but the thread it leaves is work-hardened and, in aluminum especially, measurably stronger than a cut thread.
Thread milling works on a different principle. A thread mill is a smaller cutter with the thread form ground onto its teeth; the machine helical-interpolates it around the hole, spiraling down while feeding in a continuous milling cut. Because the cutter is smaller than the hole, a single tool can cut a range of diameters at its ground pitch, and it can produce right-hand or left-hand threads, internal or external, with the same tool. The trade is cycle time — thread milling is slower per hole than tapping — and that is the cost most shops weigh first.
Blind holes and depth: where taps run out of room
The tap's structural weakness is the blind hole, and the deeper the hole, the worse it gets. Chips in a blind hole have nowhere to go except back up the flutes, so they pack ahead of the cutting edges, the torque spikes, and the tap snaps. Spiral-flute taps and pecking cycles help, but every reversal at the bottom of a deep hole is a stress cycle on a brittle, hardened tool that is exactly the diameter of the thread it is cutting.
Thread mills do not fight the same battle. The cutter is smaller than the hole, so chips fall away into the clearance around it and flood coolant can reach the cut directly. There is no reversal at the bottom: the mill spirals in, cuts, and spirals back out in the same continuous motion, and it can generate a full thread right down to the bottom of a blind hole with only a small runout allowance. A practical line that comes out of a lot of shops is that beyond roughly 2.5 to 3 times the diameter in depth, thread milling stops being a luxury and starts being the reliable option. Shallower than that, in an open hole, tapping is usually the faster and cheaper call.
Material and chip control decide the physics
The material dictates which method wins on chip control, and chip control is where most thread failures actually happen. In 6061 aluminum, both methods run well. Tapping is blindingly fast, and form taps shine here because they produce no chips at all and leave a stronger, work-hardened thread. Thread milling aluminum is also clean and gives a slightly better surface finish, but it costs cycle time.
The picture flips in stainless steel, titanium, and nickel alloys. These materials are gummy and work-hardening; a cut tap tears the material, the stringy chip welds to the cutting edge, and the tap loads up and snaps without warning. A thread mill, by contrast, is a milling cut with positive shear and a sharp, well-cooled edge that is only ever engaged with a fraction of the circumference. It evacuates the chip as it goes and does not pack the flutes. That is why thread milling is the default answer the moment a print calls out 316L, Ti-6Al-4V, or Inconel, even for holes that are not especially deep.
There is a middle case worth knowing: form taps can work in some stainless grades, but the forming torque is high and the material's tendency to spring back means the resulting thread can be undersized. When a stainless job lands, the safer engineering decision is almost always to thread mill it and avoid discovering the problem on a finished part.
Tool life, breakage, and the real cost of a broken tap
The two methods fail in very different ways, and the difference shows up on the balance sheet. A tap fails suddenly. It wears, the torque climbs, and then it snaps flush in the hole — often on the final hole of a long run, often in a part that already had three other operations completed. A broken tap in a finished part means either burning it out with an EDM (hours, and a machine you may not have) or scrapping the part entirely. The tap itself cost four dollars; the scrap it caused cost fifty.
A thread mill wears gradually. The cutting load climbs in a predictable curve, so tool-life management can flag it for replacement before it fails, and if it does break, it is smaller than the hole it is cutting and usually extracts without wrecking the thread. That predictability is worth real money in lights-out or high-volume work, where an unattended tap break is how an entire pallet of parts becomes scrap by morning.
"We stopped tapping anything deeper than 2.5 times diameter in stainless. The math was simple: one broken tap costs an hour of EDM and a scrapped block, while a thread mill costs a little more per hole and wears out where you can see it coming. Predictability beats a cheap tool every time."
Thread size, position, and surface finish
Beyond breakage, the two methods differ in how precisely they can hold the thread itself. A tap is a fixed tool: whatever pitch diameter it is ground and honed to, that is what the hole gets, and as the tap wears that diameter drifts. You can buy taps for a Class 2 or Class 3 fit, but you cannot dial in a correction mid-run the way you can with a mill.
Thread milling, because it is interpolated, gives the programmer direct control over the pitch diameter through a tool offset. That means you can hold a tight fit class, compensate for tool wear across a long production run, and correct a thread that measures slightly off without switching tools. Position control is better too: a thread mill tracks the machine's positioning accuracy, while a tapped thread follows wherever the pre-drilled hole ended up, so any drill wander is inherited by the thread.
Surface finish is the quieter advantage. In tough or gummy material, a tapped thread is a torn, smeared surface, while a thread milled thread is a clean shear cut that accepts plating, coating, and gaging more consistently. For parts that will be anodized, passivated, or checked with a go/no-go gage on a tight spec, the milled thread is the one that inspects cleanly.
Choosing between them without guessing
The decision is mostly a function of four variables: depth, material, batch size, and what a scrapped part costs. Work through them in order and the ambiguity tends to disappear. For a quick side-by-side, the table below summarizes how the two methods stack up on the dimensions that actually matter on the floor.
| Parameter | Cut Tapping | Form Tapping | Thread Milling |
|---|---|---|---|
| Cycle time per hole | Fastest | Fastest | Slowest (interpolated) |
| Tool cost | $ | $ | $$–$$$ (one tool, many sizes) |
| Practical depth limit | ~2.5–3× dia | ~2–3× dia | Bottom of blind hole |
| Chip evacuation | Flutes carry chips up | None (chips not formed) | Falls into clearance |
| Material range | Aluminum, steel | Ductile only | Any, incl. stainless/Ti/Inconel |
| Pitch diameter control | Fixed by tool | Fixed by tool | Adjustable via offset |
| Failure mode | Sudden snap | Sudden snap | Gradual wear |
| Broken tool recovery | EDM or scrap | EDM or scrap | Usually extractable |
| Surface finish in tough material | Torn / smeared | Work-hardened, smooth | Clean shear cut |
| Best fit | Shallow open holes, high volume | Aluminum threads, chip-free | Deep, tough material, tight class |
If the numbers feel abstract, walk the checklist instead. It covers the situations we actually see come through quoting, and each line has a clear answer.
- Hole deeper than ~2.5–3× diameter, especially blind. Thread mill. Taps break in the reversal zone.
- Material is 316L, titanium, or a nickel alloy. Thread mill. Gummy, work-hardening stock is where taps die.
- 6061 aluminum, shallow open holes, big batch. Tap it, or form tap for a stronger chip-free thread.
- Tight pitch-diameter spec or a Class 3 fit. Thread mill. You can correct the size with an offset.
- Unattended or lights-out run. Thread mill. A predictable wear curve beats an overnight tap snap.
- One thread size, thousands of parts, forgiving tolerance. Tap it. The cycle-time savings compound.
- Threads that must survive anodizing or passivation. Thread mill or form tap for a cleaner, more consistent surface.
The honest takeaway is that neither method is uniformly better. Tapping wins on speed and tool cost in the easy cases; thread milling wins on reliability, depth, and control the moment the material gets difficult or the consequences of a broken tool get expensive. If you are not sure which side of that line your part sits on, that is exactly the kind of call a good shop should make for you before the first hole is drilled.
Thread work splits across our CNC milling cells and, for small high-volume fasteners, our Swiss turning lathes.