CHX Precision Metal

Tapping, thread milling or single-point: choosing the right thread route

Updated 2026-11-15 · CHX Precision Metal

Tapping is fastest and cheapest, but a broken tap in a small hole can scrap the part. Thread milling handles large diameters and difficult materials and gives a better thread in blind holes, at three to five times the cycle time. Single-point turning is for threads on a lathe axis. The choice is driven by diameter, depth, material and how much the part costs to scrap.

The three routes

RouteTypical rangeCycle timeFailure modeBest for
Tapping (cut or form)M1.6-M16FastestTap breakage in blind holesThrough holes, ductile materials, small threads
Thread millingM6 and up3-5x tappingTool wear on the crestLarge threads, hard materials, high-value parts
Single-point (lathe)Any on-axis threadModerateThread gauge driftExternal threads on turned parts
Thread forming (roll tap)M2-M12 in ductile metalFastMaterial must be ductileAluminium, 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:

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 specifyWhy it mattersExample on the drawing
Thread class6H vs 6G changes the pitch diameter allowanceM8 × 1.25 - 6H
Depth vs full threadA tap needs 3-5 pitches of run-outM8 × 1.25 - 6H ↧12 (full thread 9)
Through or blindChanges tool selection and scrap riskTHRU or ↧
Thread reliefNeeded when the thread runs to a shoulderRelief groove 8.6 × 2
Coating / plating allowancePlating closes the threadM8 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:

RouteCycle time per holeTool cost per 200 holesScrap riskVerdict
Cut tap (spiral flute)8-12 sOne tap, ~USD 12, handles ~300 holesModerate - 304 work-hardensCheapest if the tap survives
Form tap6-9 sOne tap, ~USD 18Low in ductile material, high in 304Good for aluminium, risky here
Thread mill35-45 sOne cutter, ~USD 55, lasts 1,000+ holesNear zeroCosts 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

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