Thread Milling vs Tapping in Aluminium: When Each Wins

Tapping is three to five times faster per hole below M6 in aluminium. Thread milling wins above M10, in thin-wall or high-value parts, and in hardened material, because one broken tap can scrap a part worth hundreds; a milled thread can also be corrected or opened up without re-fixturing the part.

How much faster is tapping?

A tap cuts a thread in one pass at the thread pitch, so a 10 mm deep M6 hole is a couple of seconds of cutting. Thread milling interpolates a helix with a small single-point cutter, which means many revolutions and a much longer toolpath. In aluminium the time difference is roughly 3–5× per hole.

On a part with thirty M4 holes, tapping wins by minutes and there is no argument. The question only becomes interesting when the tap is expensive, the thread is large, or the part is worth enough that a broken tool is a catastrophe rather than an inconvenience.

When does a broken tap decide the process?

A tap breaks in aluminium for predictable reasons: chip packing in a blind hole, a hole drilled undersize, a worn tap pushed past its limit, or a part that shifted in the fixture. When that happens in a €15 bracket you remove the tap with a spark eroder or scrap the part. When it happens in a €400 machined housing, you have just spent a week of machining time.

Thread milling cannot break in the same way. The cutter is small and the load is low; if it does fail, it fails outside the thread and the operation can be repeated. For a single-point thread mill the tool is also one size for a wide range of diameters, so a tool break does not mean waiting for a special tap.

The decision is not "how fast is the thread" but "what does a broken tool cost at this point in the process".

What about thread quality and gauge life?

A milled thread is produced by a controlled helical interpolation, so pitch diameter is set by the toolpath and can be adjusted in microns by changing the cutter compensation. That makes correction possible: if a thread gauges tight on the first part, you offset and recut the same part. With tapping, a thread that gauges wrong is usually a scrap decision.

Surface finish favours milling too, particularly in aluminium where taps smear rather than cut if lubrication is marginal. The counter-argument is that a good tap in a well-set machine produces a perfectly serviceable 6H thread all day; most production tapping is fine. Milling wins on control, not on baseline quality.

Which process should a drawing specify?

Most drawings should specify the thread, not the process — 6H, depth, and the class — and let the shop choose. Specify the process only when there is a real reason:

• Threads larger than M20, where taps are special-order and expensive.
• Threads in thin walls, where tapping force distorts the wall.
• Threads that must be concentric with a bore to a tight true position, where single-setup milling avoids a second op.
• Threads in hardened material, where tapping is not viable at all.
• Threads on high-value parts late in the process, where scrap risk is unacceptable.

The reverse also applies: if the drawing says "thread mill only" on forty M4 holes in a €20 bracket, you have added cost for no benefit. Process notes should carry a reason, and a shop that asks why is doing its job.

About the author

CHX Precision Metal is a precision machining supplier in Shajing, Bao'an District, Shenzhen, founded in 2013. The floor runs 220 CNC machines — 100 five-axis machining centres (30 configured 3+2), 70 Tsugami Swiss-type lathes and 50 CNC lathes — under ISO 9001:2015 and ISO 14001:2015. Standard tolerance is ±0.005 mm, or better where the drawing requires it; prototypes ship in 3–7 working days, production in 7–15, MOQ 1 piece. Capability details: chxmetal.com