A thread is one of the few operations where a mistake cannot be put right: if a tap snaps off inside the hole, the part usually goes in the bin. Which is why it pays to be clear about the three options before deciding.
1. Tapping
A tap is a tool that already carries the form of the thread and generates it in one pass. It is the fastest method and the most used on small and medium threads.
The critical part is synchronisation: the feed has to match the pitch of the thread exactly. One spindle revolution, one pitch of feed. If it does not line up, the tap cuts where it should not, or it snaps.
Modern machines do it with rigid tapping (the G84 cycle on most Fanuc controls): the control coordinates spindle and Z axis. On machines without that capability a compensating tapping holder is used, which absorbs the mismatch with a spring.
Working out the tapping drill is where most of the mistakes happen. The quick rule for coarse metric threads:
drill Ø = nominal Ø − pitch
For an M8×1.25: 8 − 1.25 = 6.75 mm. For an M10×1.5: 8.5 mm. For an M6×1: 5 mm. If the hole is tight the tap suffers and breaks; if it is loose the thread loses flank height and strength.
Three more things that prevent breakages: plenty of lubricant made for tapping, not reaching the bottom in blind holes (leave at least two pitches of margin), and using a spiral-flute tap in blind holes so the chip comes up and out, and a straight-flute or spiral-point tap in through holes.
2. Single-point, on the lathe
This is the classic lathe method and it is still the best when the thread is large, the material is hard, or you need a profile that is not standard. The tool carries the thread profile and takes successive passes, each one deeper, with the carriage synchronised to the spindle.
It needs more passes and more time, but it has two important advantages: you control the fit — you can take one more pass if the thread comes out tight — and there is no tool to get left inside.
The passes are taken at decreasing depth, not equal: the first ones remove more and the last ones barely scrape, so the force does not grow and the finish comes out clean.
3. Helical interpolation, with a thread mill
The most modern option and the one that solves the awkward cases. The cutter is smaller than the hole and describes a helix: it turns on its own axis while following a circular path and descending by one pitch per revolution.
The advantages are considerable:
- One tool covers several diameters of the same pitch.
- If something goes wrong, the cutter comes out of the hole: it does not get trapped.
- You can adjust the effective diameter by changing the radius of the path, so you correct a tight thread without changing tools.
- It works well in hard materials, in stainless, and on large threads where a tap would demand enormous torque.
The drawback is that it is slower and it needs a machine with helical interpolation and a properly written program. For M6 fasteners in production it does not pay; for an M30 in stainless, it does.
Which one to choose
- Small threads in production, forgiving material: tapping, rigid if the machine allows it.
- External thread on the lathe, or a special profile: single-point.
- Large threads, stainless, titanium, high-value parts: thread milling.
- Blind hole with little clearance at the bottom: thread milling, because it reaches lower than a tap.
Why taps break
Almost always one of these five: a tapping drill that is too small, lack of lubrication, chip packed into a blind hole, misalignment between tap and hole, or bottoming out. None of them is bad luck; all five are controlled beforehand.
And once it has broken
If the broken piece sticks out, needle-nose pliers and patience. If it is flush or below, a tap extractor or sinker EDM, which is what a specialist shop does and the reason many workshops in the directory offer EDM as a service. Never try to drill it out: the tap is harder than the drill.
Need a part machined? The directory of Spanish machine shops lists more than 700 workshops across Spain with their processes, materials and certifications verified, filterable by province. And if you are learning, the CNC Path takes you from G-code to your first part.