Thread milling guide

CNC Steps: How to Thread Mill on a CNC Machine

Thread milling replaces tapping when the hole is large, the material is tough, or the part cannot be scrapped. This guide walks through the CNC steps from tool selection to final gage check, with the parameters and mistakes that matter on the shop floor.

Get Instant Quote Talk to an Engineer

Ø6–300 mm threadsRight and left handSingle-point and multi-fluteGage-checked

On this page

Key takeaways

Thread milling beats tapping on large holesA single-point mill cuts any diameter above Ø6 mm with one tool, so you stop stocking a tap for every size.

Helical interpolation is the core motionThe cutter orbits while descending one pitch per revolution, so the thread form comes from the path, not the tool tip.

Climb milling gives the cleanest flankCutting downhill on the flank leaves a better finish and less burr than conventional direction on most steels.

Feed rate is programmed at the cutter centerlineThe edge travels faster than the center on an orbit, so the feed you type is not the feed the insert sees.

Gage the pitch diameter, not the crestA thread can look perfect and still fail a go/no-go check if the pitch diameter is off by 0.05 mm.

Section 1

When thread milling makes sense

Tapping is fast and cheap when the hole is small, the material is free-cutting, and the part is low value. Thread milling earns its place when any of those conditions breaks down. A tapped hole that snaps a tap usually scraps the part, because the broken tool is harder than the workpiece and rarely comes out clean.

Thread milling suits holes above roughly Ø6 mm, blind holes where chip evacuation is awkward, and materials that work-harden. Stainless 316, 17-4PH, Inconel, and titanium all tend to grab a tap. A milled thread is cut with an interrupted edge, so the tool does not load up the same way and chips clear through the helix.

The method also pays off on prototypes and low-volume runs. One single-point tool covers a range of diameters and both hand directions, which removes the tap inventory problem entirely. On a 10,000-part run, a form tool with multiple flutes is usually faster per hole, but a single-point tool is still the safer first article.

One more case: thin-wall parts and large diameters. Tapping a Ø40 mm hole in a thin aluminum housing puts high torque into the wall and distorts the bore. A helical mill applies a much smaller radial load and leaves the wall round. That is often the deciding factor, not cycle time.

1
Hole above Ø6 mmBelow that, a tap is usually faster and cheaper.
2
Blind holesChips fall into the helix instead of packing ahead of the tool.
3
Work-hardening alloysStainless, titanium, and nickel alloys grab taps.
4
Thin wallsLower radial load keeps the bore round.

Section 2

Pick the right thread mill for the job

Three families cover most work. A single-point or single-flute mill looks like a small boring bar with one insert or one ground tooth. It cuts any pitch within its range, cuts right and left hand, and cuts internal or external, all with the same tool. It is the most flexible option and the slowest per hole.

A multi-flute form mill has the full thread profile ground into several teeth. It cuts the complete thread in one 360° orbit, so cycle time drops sharply. The trade-off is that each tool is tied to one pitch and often one diameter range. On high-volume aluminum and steel parts, that trade is worth it.

Solid carbide tools hold their edge longer in stainless and hardened steel, but they chip if the setup is not rigid. Indexable tools cost more up front and cut a slightly less crisp flank, yet a broken insert is a two-minute fix instead of a re-machining job.

For threads above Ø25 mm, an indexable single-point tool is often the practical choice. Cutting forces grow with diameter and depth, and a solid tool in that size gets expensive to replace. Also check the shank diameter against the hole: the tool body must clear the minor diameter through the whole helix.

1
Single-pointAny pitch, both hands, best for prototypes and odd sizes.
2
Multi-flute formOne orbit per thread, best for volume.
3
Solid carbideSharper flank, suited to stainless and hardened steel.
4
IndexableCheaper to replace, practical above Ø25 mm.

Section 3

Set the helix, the speed, and the feed

The helix is the heart of the cut. The tool orbits at the thread radius and descends exactly one pitch per full revolution. On most controllers this is a G02 or G03 arc with a Z increment, or a G12/G13 circular pocket cycle with a Z step. If the pitch increment is wrong, the thread gage will not enter, regardless of how good the tool is.

Cutting speed depends on material and tool coating. In aluminum 6061, run 150–250 m/min surface speed. In 4140 steel, 90–150 m/min. In 316 stainless, 60–100 m/min. In titanium and Inconel, stay at 30–60 m/min and accept the slower cycle. These are starting points, not limits; listen to the cut and adjust.

Feed rate on the orbit is not the same as the feed at the cutting edge. The edge travels on a larger radius than the tool center, so the programmed feed must be scaled by the ratio of the two. Many CAM systems handle this automatically. If you hand-write the code, calculate it or the flutes will rub instead of cut.

Use climb milling on the flank for a cleaner finish in steel and stainless. Conventional direction can work in aluminum where the tool tends to pull in. Either way, take a roughing pass and a finishing pass. One pass at full depth overloads a small tool and leaves a torn crest.

1
One pitch per revThe Z step must equal the thread pitch exactly.
2
Speed by material150–250 m/min aluminum, 60–100 m/min stainless.
3
Scale the feedProgrammed centerline feed is not the edge feed.
4
Two passesRough then finish, especially on small tools.

Section 4

Chip control and coolant

Thread milling makes a long, stringy chip that wants to wrap around the tool shank. In a blind hole, that chip has nowhere to go. Use through-spindle coolant if the machine has it, aimed down the helix, so chips flush out ahead of the tool. Without it, program a retract and a blow-off between passes.

Air blast works well in aluminum and cast iron where coolant is messy or not wanted. In stainless and titanium, high-pressure coolant does two jobs: it clears chips and it keeps the edge cool, which slows work hardening. Flood coolant alone is often not enough in a deep blind hole.

Watch the first hole. If chips are packing, reduce the Z step per pass and add an extra orbit. If the finish looks smeared, the tool is rubbing rather than cutting, which usually means the feed is too low or the speed is too high for the material.

Never let the tool dwell at the bottom of a blind hole. A short pause is enough to rub the flank and work-harden the crest. Keep the tool moving and retract on the same helix.

1
Through-spindle coolantBest chip evacuation in blind holes.
2
Air blastClean option for aluminum and cast iron.
3
No dwellPausing at depth rubs the flank and hardens the crest.
4
Reduce Z stepSmaller step per orbit if chips pack.

Section 5

Common mistakes and how to catch them

The most common failure is a wrong pitch increment in the helix. The thread looks fine to the eye and the gage will not start. Check the code before the first cut: one revolution must equal one pitch of Z travel. On a 1.5 mm pitch thread, four revolutions must move 6.0 mm in Z.

Second is tool runout. A thread mill with 0.02 mm of runout cuts an oversize thread on one flank and an undersize thread on the other. Indicate the tool in the holder before the run. If runout is above 0.01 mm, reset the holder.

Third is feed scaling. If the programmed feed is not corrected for the orbital radius, the tool rubs and the insert wears on the flank within a few holes. The symptom is a polished, shiny flank and a poor finish. Fix the feed, not the speed.

Fourth is gauging the wrong feature. Measure the pitch diameter with a thread gage or a three-wire setup, not the crest. A thread can look right and still fail because the pitch diameter is 0.05 mm off. We inspect 100% of threaded features before shipment for this reason.

1
Pitch incrementOne revolution equals one pitch of Z travel.
2
Runout under 0.01 mmIndicate the tool in the holder before cutting.
3
Feed scalingUncorrected feed rubs the flank and wears the insert.
4
Pitch diameterGage the pitch diameter, not the crest.

Step by step

Seven CNC steps for a clean thread

Follow in order. Each step lists the parameter range and the mistake to avoid.

1
1. Check the drawing for thread calloutConfirm nominal diameter, pitch, class, and hand. On a 1/4-20 UNC internal thread, the minor diameter is about 5.35 mm, so the tool shank must be smaller. Avoid starting without the class: 2B and 3B need different pre-drill sizes.
2
2. Choose the tool and verify clearancePick a single-point mill for odd sizes or a form mill for volume. Check that the tool body clears the minor diameter through the full helix depth. A tool that rubs the hole wall will break on the first orbit.
3
3. Indicate the toolMeasure runout on the flutes with a dial indicator. Keep it under 0.01 mm. Reset or replace the holder if it is worse. This single check prevents most oversize threads.
4
4. Program the helixUse G02 or G03 with a Z increment equal to one pitch per revolution. For a 1.5 mm pitch, four revolutions move 6.0 mm in Z. Use climb direction in steel and stainless. Avoid a wrong Z increment; the gage will not enter.
5
5. Set speed and feedStart at 150–250 m/min for aluminum 6061, 90–150 m/min for 4140 steel, 60–100 m/min for 316 stainless, and 30–60 m/min for titanium. Scale the feed for the orbital radius. Avoid running the un-scaled centerline feed on the edge.
6
6. Cut a roughing pass, then a finishing passTake the roughing pass at about 60% of the radial depth, then finish to size. In a blind hole, use through-spindle coolant or air blast and never dwell at the bottom. Avoid a single full-depth pass on small tools.
7
7. Gage the pitch diameterUse a go/no-go gage or a three-wire measurement on the pitch diameter. Record the result. Avoid judging the thread by eye or by the crest; a good-looking thread can still fail the gage.

Decision table

Thread milling compared with tapping

Pick the process before you pick the tool.

Factor	Thread milling	Tapping
Hole size	Ø6 mm and above	Any size, best under Ø6 mm
Tool per size	One tool covers many diameters	One tap per size and pitch
Broken tool risk	Tool breaks, part usually survives	Broken tap often scraps the part
Chip evacuation	Chips clear through the helix	Chips pack in blind holes
Thin-wall parts	Low radial load, bore stays round	High torque, wall distorts
Cycle time	Slower per hole on single-point	Faster per hole
Best for	Prototypes, tough alloys, large holes	Volume, free-cutting, small holes

Thread milling is a process choice, not an upgrade

If the hole is under Ø6 mm, the material is free-cutting, and the part is cheap, tap it. For large holes, tough alloys, thin walls, and blind holes, the CNC steps above give you a thread that passes the gage the first time.

Get Instant Quote Talk to an Engineer

FAQs

Thread milling questions engineers ask

Can a single thread mill cut both right-hand and left-hand threads?

Yes. The direction is set by the helix in the program, not by the tool. A single-point mill cuts internal and external threads in either hand as long as the shank clears the hole.

That is the main reason single-point tools are kept on hand for prototypes and repair work. One tool replaces a shelf of taps.

What tolerance can thread milling hold?

On our machines, thread milling holds ±0.005 mm on the pitch diameter when the tool is indicated under 0.01 mm and the feed is scaled correctly. That meets most 2B and 3B class requirements.

The limit is usually tool runout and thermal growth, not the machine. Check the tool in the holder before blaming the program.

How do I handle a blind hole without a thread relief?

Program the helix to stop short of the bottom and leave room for the chip. Use a tool with a short flute length so the shank does not rub the crest above.

If there is no relief groove, the thread fades out at the bottom. Tell the designer; a relief of one to two pitches makes the cut far more reliable.

Why does my thread gage enter only partway?

Almost always a wrong pitch increment in the helix, or a tool runout problem. Check that one revolution equals one pitch of Z travel, then indicate the tool.

A third cause is a worn insert cutting an undersize pitch diameter. Swap the insert and re-cut one test hole before running the batch.

Does thread milling work in titanium and Inconel?

Yes, and it is often the better choice because the cut is interrupted and the tool does not load up the way a tap does. Run 30–60 m/min with high-pressure coolant.

Keep the Z step small and take a finishing pass. Work hardening on the crest is the main risk, so never let the tool dwell at depth.

How do I check the thread on the shop floor?

Use a go/no-go gage for the class called out on the drawing, or a three-wire measurement for the pitch diameter. Record the reading against the part number.

We inspect 100% of threaded features before shipment and can supply reports on request.

Send us your threaded part

Upload a drawing and we return a quotation with a free DFM analysis within 12 hours. Threads are gaged before shipment, and your files stay confidential under NDA on request.

12-hour quoteNo minimum order100% inspectionNDA on request

Get Instant Quote Talk to an Engineer

Follow our shop