Threads look like a solved problem until a shop quotes them. Then you learn that a 1/4-20 hole in the bottom of a deep pocket can double the price of an otherwise simple aluminum part. Tapping and thread milling both make threads, but they fail in different ways, and knowing which failure mode matters for your part is worth more than any catalog.
The two processes, in one paragraph each
Tapping uses a forming or cutting tap driven straight into a pre-drilled hole. It is fast — a M6 tap in aluminum runs in a second or two — and every standard CNC metal machining shop does it daily on tapping heads or rigid tapping spindles. The catch: the tap is basically a non-repairable, form-matching tool. If it goes in crooked, binds, or hits hardened material, it usually breaks in the hole, and extracting a broken tap from a finished part is the kind of afternoon nobody bills for.
Thread milling uses a small single-profile or full-profile end mill that helically interpolates the thread. The tool diameter is smaller than the hole, so nothing can jam in a way that breaks the part. You control the pitch exactly, you can adjust the thread size in 0.01 mm increments by changing the cutter radius compensation, and one tool can cut left-hand, right-hand, and multiple depths. The trade is cycle time: interpolation takes 3–10× longer than tapping, and it needs a 3-axis interpolation-capable machine with decent helical accuracy.
Where tapping still wins
- Blind holes in aluminum, steel, and ADC12. For M5–M12 (and #8–1/2" UNF) in gummy, forgiving materials, a spiral-flute tap at the right speed is unbeatable on cost. On 6061-T6 a good coated spiral tap will run thousands of holes.
- High volume. If your bracket has 8 × M6 holes and you're making 500 of them, thread milling adds real money per part.
- Small holes, generally below M4 / #6. Micro thread mills exist, but the tools get fragile and the cycle-time penalty grows; most shops tap anything under ~3 mm.
- Loose tolerance threads. A tapped 6H thread is what the process gives you, and for most brackets that's exactly right.
Where thread milling earns its keep
The list of jobs that should be thread milled is surprisingly consistent across shops:
- Deep or hard materials. Tapping Inconel, 17-4 at 40 HRC, or A2 at 50+ HRC is a coin flip. Thread milling with a carbide cutter takes it easy and predictable.
- Large diameters. Above roughly M16 or 5/8", taps get big, expensive, and torque-hungry. A thread mill handles M24 or a 1-1/4" NPT with the same small tool.
- Interrupted or cross holes. If a cross-drilled hole intersects the thread, a tap will snag. Thread mills shrug at interruptions.
- Tight position and perpendicularity. Because the thread is generated by interpolation off the machine's path, the thread follows the hole position exactly. Taps self-feed and can be pushed off-axis in deep holes.
- Blind holes where full-bottom threads matter. Thread mills can cut closer to the bottom (typically within 0.5–1× pitch) than a tapered-entry tap.
- Rework. Oversize a tapped hole 0.1 mm and a thread mill can cut a slightly larger pitch diameter to salvage the part — tapping has no such second chance.
A useful rule of thumb from prototype work: if the part costs more than about $100 when scrapped, thread mill anything above M8. The cycle-time penalty is a few dollars; a scrapped machined body is not.
Design details that decide the outcome
Depth rules
Blind-hole threads need relief. Specify usable thread depth, not tap-drill depth. For aluminum, 1.5–2× diameter of full thread engagement carries essentially all the load a bolt can deliver; going deeper mostly adds tapping risk. In steel, 1–1.5×D is usually plenty. Ask for a chamfer or a bottom relief groove — a tap that bottoms out on unthreaded stock will break no matter how good the program is.
Materials
6061-T6 taps beautifully; 7075-T6 is slightly more abrasive on taps but fine. Die-cast alloys like ADC12 and A380 tap well but leave hard oxide inclusions that chip small taps — consider forming taps in silicon-free alloys or thread milling in castings with heavy skin. In stainless (304/316), galling is the enemy: spiral-point or spiral-flute taps with good lube, or just thread mill it and stop arguing with physics.
Callouts
Don't specify a class 5 interference fit unless the mating fastener is actually controlled. A 6H/2B tapped hole with a standard bolt is what 95% of prototypes need. And avoid calling out a thread on a curved or angled surface without a spotface — starting a tap off a sloped face is the #1 cause of crooked and broken taps we see in incoming drawings.
What this means for your quote
When you send a part for CNC machining, the thread strategy is one of those invisible cost lines. A design with twelve M10 × 20-deep blind holes in 6061 is a tapping job — cheap. The same twelve holes in 15-5PH stainless, cross-drilled, with class 3 threads, is a thread-milling job, and quoting it as tapping is how shops lose money or lose parts. If your drawing puts threads in any of the "thread mill" categories above, expect the shop to ask — or better, note the tricky ones on the drawing so the process is planned up front.
Threads also interact with downstream work. If a casting is going to be finished by die casting plus machining, decide whether threads get cut in the casting blank or after finish machining; doing them after the second op usually gives better position. And if the same part family might move to plastic — where molded threads replace machined ones entirely — keeping thread specs simple now makes that transition cheaper later.
Bottom line: tapping for the ordinary, thread milling for the awkward. When in doubt, send the drawing and ask which the shop intends to use — a good answer usually predicts a good part.
