Tapping, thread milling or single-point: choosing the right thread route
The three routes
| Route | Typical range | Cycle time | Failure mode | Best for |
|---|---|---|---|---|
| Tapping (cut or form) | M1.6-M16 | Fastest | Tap breakage in blind holes | Through holes, ductile materials, small threads |
| Thread milling | M6 and up | 3-5x tapping | Tool wear on the crest | Large threads, hard materials, high-value parts |
| Single-point (lathe) | Any on-axis thread | Moderate | Thread gauge drift | External threads on turned parts |
| Thread forming (roll tap) | M2-M12 in ductile metal | Fast | Material must be ductile | Aluminium, low-carbon steel, no chips |
The numbers are not hard limits. A skilled shop taps M20 in aluminium every week. The table is about where each route stops being the economical default.
Why a broken tap is worse than it looks
A tap breaks in a blind hole. Now you have a hardened HSS or carbide spiral inside a part that may already have 20 minutes of machining in it. Options: spark erosion (slow, needs a machine and an operator), drilling it out (risks damaging the thread flanks), or scrap the part.
For a part that costs 3 yuan, scrapping is fine. For a part that has been through five-axis milling, heat treatment and anodising, thread milling - which cannot break - is cheaper in expectation even at four times the cycle time.
Thread milling, in practice
A thread mill is a small multi-tooth cutter that helical-interpolates the thread. Three advantages beyond not breaking:
- One tool, many diameters. A single M6-M12 thread mill covers the range a shop would need six taps for.
- Better thread in blind holes. The tool can cut to within half a pitch of the bottom, where a tap needs run-out space.
- Correction possible. If the thread is undersized, the tool can be offset and the thread re-cut. A tap cannot.
The cost is cycle time and tool cost. For a 400-piece run of M8 through holes in aluminium, tapping is the right answer and thread milling is 4x the machine time for no benefit. For 20 pieces of M16 in 17-4PH, thread milling wins on both scrap risk and thread quality.
Specifying threads so nothing is guessed
A drawing that says "M8" leaves three decisions to the shop: thread class, depth, and whether it is a through or blind hole. All three change the outcome.
| What to specify | Why it matters | Example on the drawing |
|---|---|---|
| Thread class | 6H vs 6G changes the pitch diameter allowance | M8 × 1.25 - 6H |
| Depth vs full thread | A tap needs 3-5 pitches of run-out | M8 × 1.25 - 6H ↧12 (full thread 9) |
| Through or blind | Changes tool selection and scrap risk | THRU or ↧ |
| Thread relief | Needed when the thread runs to a shoulder | Relief groove 8.6 × 2 |
| Coating / plating allowance | Plating closes the thread | M8 6H, plated after - allowance per note 4 |
The plating allowance line is the one that gets missed. A zinc-plated M8 6H thread will not accept a 6H gauge after plating, because the coating reduces the pitch diameter. Either plate-then-tap (only possible for some coatings) or run the thread oversize and specify the allowance.
Gauging
Threads are gauged with GO/NO-GO plug or ring gauges, not with calipers and not with a screw from the assembly bench. The GO gauge must enter the full thread length by hand; the NO-GO must not enter more than 1.5 turns. For plated threads, gauge after plating.
If the inspection report lists threads as "checked with mating screw", that is a fit check, not a conformity check. Ask for gauge results on the dimensions that matter.
A worked cost comparison
M10 × 1.5, blind hole 20 mm deep, 304 stainless, 200 pieces. Three routes:
| Route | Cycle time per hole | Tool cost per 200 holes | Scrap risk | Verdict |
|---|---|---|---|---|
| Cut tap (spiral flute) | 8-12 s | One tap, ~USD 12, handles ~300 holes | Moderate - 304 work-hardens | Cheapest if the tap survives |
| Form tap | 6-9 s | One tap, ~USD 18 | Low in ductile material, high in 304 | Good for aluminium, risky here |
| Thread mill | 35-45 s | One cutter, ~USD 55, lasts 1,000+ holes | Near zero | Costs more cycle time, saves scrap |
On 200 holes the difference between tapping and thread milling is about 80 minutes of spindle time. If one tap breaks in a part that already carries 25 minutes of machining, the scrap cost exceeds the saved time. Above roughly USD 8-10 of value per part, thread milling is the cheaper route even though it looks slower.
Blind holes: the run-out problem
A cut tap needs 3-5 pitches of run-out below the full thread depth, because the chamfer at the tap tip has to go somewhere. A thread mill needs about half a pitch. On a 20 mm deep M10 blind hole with 15 mm of full thread, a tap needs 22-27 mm of drill depth; a thread mill needs 16 mm.
That difference matters when the hole depth is limited by a wall thickness. It is also why drawings that specify "full thread to bottom" are unrealistic - no process delivers a full thread to a flat bottom in a blind hole.
What to check on the inspection report
- GO gauge enters the full thread length by hand, without a wrench.
- NO-GO gauge enters no more than 1.5 turns.
- Thread depth measured, not assumed from the drill depth.
- For plated parts, gauged after plating - the coating closes the pitch diameter.
Questions buyers ask
Can you tap stainless steel without breaking taps?
Yes, with the right tap (spiral flute for blind holes, form tap for ductile grades), correct lubricant, and peck tapping on deep holes. 304 work-hardens, so a tap that rubs instead of cutting will fail - the feed has to keep it cutting.
Why is my M3 thread stripping?
Usually insufficient engagement depth in aluminium, or a thread that was formed rather than cut in a material that work-hardened. Rule of thumb: engagement depth 2x diameter in aluminium, 1.5x in steel.
Does thread milling work on a 3-axis mill?
Yes, it needs helical interpolation and a thread mill, not a fourth axis. Most modern 3-axis machines can do it.
How much does thread milling add to the price?
Cycle time is typically 3-5 times tapping for the same thread, which on a small thread in a short cycle can mean 10-20% on the part price. On a large thread in a hard material it can be neutral, because tapping would need multiple tools and a slower spindle.
Threads, tolerances and inspection scope on the main site are written per drawing, not per catalogue.
equipment list