Thread milling: the feed you program is not the feed that cuts

Two circles, not one

In thread milling, the tool follows a helix: it spins on its own axis while describing a circle around the hole axis, rising or falling by the thread pitch.

The important point is that two different radii are turning at once:

• The tool centre follows a circle of radius (D_thread − D_cutter) / 2
• The cutting edge follows a circle of radius D_thread / 2

Both complete the revolution in the same time. If two points complete the same revolution in the same time but one is further from the centre, that one moves faster. Always.

The relationship

cutting-edge speed        D_thread
──────────────────  =  ───────────────────
centre speed             D_thread − D_cutter

Put in the numbers for a normal case. An M3 thread with a Ø2.4 thread mill:

    3
─────────  =  5
 3 − 2.4

Five times. The cutting edge travels at five times the speed of the point you programmed.

Here is what makes this a real trap: the relationship does not depend on thread size, only on the proportion. With the cutter at 80% of the diameter, it is 5× in M3 and M10 alike. What worked on a large thread can still fail in the same way on a small one.

Look at the curve. Between 50% and 70%, the error is tolerable. From 80% upwards it takes off. Commercial thread mills often sit right there, because a larger cutter is stiffer and gives a better profile.

The tool that threads best is the one that penalises your feed the most.

What happens in practice

If you program the centre feed as though it were normal contouring, the actual chip thickness at the cutting edge is several times what you intended. The cutter:

• Survives in soft material and at shallow depth. That is why it works “almost always”.
• Suffers silently through many threads, with accelerated wear you attribute to the material or tool batch.
• Breaks when slightly harder material, an already worn cutter or a deeper thread coincide.

And because it breaks inside a hole in a part that already has hours of machining in it, the shock is expensive.

The correction

First decide the feed you want at the cutting edge — from chip load and number of flutes — then program at the centre:

centre_feed = edge_feed × (D_thread − D_cutter) / D_thread

Using the earlier example, for 300 mm/min at the edge on an M3 thread with a Ø2.4 cutter:

300 × (3 − 2.4) / 3 = 60 mm/min

Sixty, not three hundred. The difference between those numbers is the difference between threading and breaking.

Check one thing before changing anything

Find out which feed your CAM outputs.

Some systems output tool-centre feed; others allow it to be referenced to the contact point. If yours already compensates and you also correct it manually, the feed becomes absurdly slow: rubbing instead of cutting, another way to damage a tool.

How to know without guessing: program a thread, inspect the generated code and compare the feed value with the one you entered in the operation. If they match, it is not compensating and the correction is yours. If the output is lower, it is already doing it.

Do it once, write it down and stop thinking about it.

The same effect elsewhere

This relationship between centre radius and cutting-edge radius appears whenever you interpolate a circle with a tool that is not small relative to the diameter:

• Interpolating a hole with a cutter close to the hole diameter.
• Contouring a small internal radius with a similarly sized cutter radius. Here the effect is reversed and matters too: the edge travels slower than the centre, the contact arc increases and heat builds up.
• Machining a circular chamfer with a large tool.

The mental rule for all these cases: the feed that matters is at the cutting edge, not at the tool centre. CAM lets you program the latter. You need to think about the former.

At 7Axis Industrial we design and manufacture custom parts, tooling and equipment. Machining judgement is part of the job, not an addition.

Parts, spares and short runs →