CNC knowledge

Three Ways to Treat Threads for the CNC Machining Center

Threads give more trouble than any other feature on a milled or turned part. This guide covers the three practical ways to treat threads for the CNC machining center: rigid tapping, thread milling, and single-point turning. You will see which method fits which hole size and material, what parameters to start from, and where each one fails.

Get Instant Quote Talk to an Engineer

Rigid tappingThread millingSingle-point turning

Three ways to treat threads for the CNC machining center on a machined part

On this page

Key takeaways

Tapping is fastestBest for holes from M2 to about M16 where the tap can reach and chip evacuation is not a problem.

Thread milling wins on sizeOne tool covers a range of diameters, and it cuts threads larger than any tap you can hold in an ER32 collet.

Turning is for round partsExternal and internal threads on shafts and bushings come off the lathe in one pass with a single-point insert.

Check the minor diameter firstMost broken taps come from an undersized pilot hole, not from a wrong feed rate.

Fit class drives the allowance6H and 6g are the common defaults; a coating or plating adds roughly 0.01 mm to the flank.

Method 1

Rigid Tapping Threads for the CNC Machining Center

Rigid tapping is the default for holes from M2 up to about M16. The spindle encoder locks the tap to the programmed feed, so the thread pitch is set by the machine, not by a floating holder. On a machining center with rigid tapping, set the feed at pitch × spindle speed and keep the speed constant through the whole cycle.

The pilot hole decides whether the tap survives. For a 6H internal thread, drill the minor diameter from the table or from the tap manufacturer's data. An M6 × 1.0 tap wants roughly 5.0 mm in aluminium and 5.1 mm in 304 stainless. Too small and the torque spikes. Too large and the thread fails a go/no-go gauge.

Use a spiral-flute tap for blind holes and a spiral-point tap for through holes. Form taps are the better choice in aluminium, copper, and mild steel because they push material instead of cutting it, so there are no chips to jam in a blind hole. Form tapping needs a slightly larger pilot hole and more spindle torque.

Start conservative. In 6061 aluminium, 300–600 rpm is a safe starting range. In 304 stainless, drop to 100–200 rpm and use plenty of cutting oil. Watch the spindle load meter on the first few holes; a steady climb means the pilot is undersized or the tap is dull.

1
Best forM2–M16 blind and through holes, high hole count, short cycle time
2
Watch outChip packing in deep blind holes and tap breakage on the reverse pass
3
CoolantFlood or through-spindle is better than mist for stainless

Method 2

Thread Milling Large or Awkward Threads

Thread milling uses a single-point or multi-tooth cutter that orbits the hole while the Z axis moves one pitch per revolution. One tool can cut a range of diameters, so you do not need a tap for every size on the drawing. That matters on a job with M20, M24, and M30 holes in the same part.

The method also handles threads that a tap cannot reach. Large diameters, threads close to a shoulder, and holes in thin walls are all easier with a mill. Because the cut is interrupted, the tool loads and unloads, so power demand stays low even in Inconel or Ti-6Al-4V.

Set the feed per tooth from the cutter data and keep the radial depth light. A typical pass is 0.1–0.3 mm radial in aluminium and 0.05–0.15 mm in stainless. Run two or three passes for coarse pitches instead of one heavy pass. Climb milling gives a cleaner flank than conventional milling.

Thread milling does take longer per hole than tapping. On a part with 40 M6 holes, tapping usually wins on cycle time. Use milling where size range, reach, or material hardness makes tapping risky. Check the thread with a go/no-go gauge, because the orbit diameter is easy to set wrong by a few hundredths.

1
Best forM16 and larger, near-shoulder threads, hard alloys, mixed sizes on one part
2
Watch outLonger cycle time and a wrong orbit radius that still looks like a thread
3
ToolingSolid carbide or indexable thread mills with internal coolant

Method 3

Single-Point Turning and Thread Milling on the Lathe

Round parts usually get their threads on the lathe. A single-point insert cuts external threads on shafts and internal threads in bushings with the same setup that turned the outside diameter. That keeps the thread concentric to the bearing journal, which a milled thread cannot promise.

Turn the major diameter to the class allowance before threading. For a 6g external thread, the major diameter runs a little under nominal. For 6H internal, the minor diameter runs a little over. Get these right and the pitch diameter lands in the middle of the tolerance band.

Set the spindle speed from the surface speed: 150–250 m/min in aluminium and 60–100 m/min in 304 stainless. Use a 29–30° infeed angle for a standard 60° insert and take several passes with a finishing pass of 0.05–0.1 mm. Spring passes clean up the flank without cutting more material.

Thread milling on a mill-turn center is the option when the part has both milled features and a large thread. It avoids a second setup, which protects position tolerance. If the thread is under M16 and the part is round, single-point turning is still the simpler route.

1
Best forShafts, bushings, fittings, any thread that must run concentric to a turned diameter
2
Watch outWrong major or minor diameter, and chatter on long unsupported shafts
3
SupportUse a tailstock or steady rest when the length-to-diameter ratio passes 4:1

Working sequence

Step by Step: Choosing and Cutting the Thread

Run these in order before the first cut

1
Read the thread calloutNote diameter, pitch, class, and whether the thread is internal or external. A callout like M8 × 1.25 6H tells you the minor diameter target and the gauge that will be used.
2
Pick the method by size and reachUnder M16 with clear access, tap. M16 and over, near a shoulder, or in a hard alloy, thread mill. On a round part with a concentric requirement, single-point turn.
3
Calculate the pilot or major diameterUse tap manufacturer data for tapping. For turning, set the major diameter to the 6g allowance and the minor to the 6H allowance. Write the numbers on the setup sheet.
4
Drill or turn to size, then checkMeasure the pilot with a pin gauge or the major with a micrometer. A 0.05 mm error here shows up as a gauge failure later.
5
Set conservative speeds for the first part300–600 rpm tapping in aluminium, 100–200 rpm in 304. Thread milling at 0.1–0.3 mm radial in aluminium. Turning at 150–250 m/min in aluminium.
6
Cut one thread and gauge itRun a go/no-go gauge on the first part, not the tenth. If the no-go enters more than two turns, the pitch diameter is oversize.
7
Adjust and recordChange one variable at a time, then log the final speed, feed, and tool number so the next run starts from a known point.

Method selection

Tapping vs Thread Milling vs Single-Point Turning

Match the method to hole size, part shape, and material

Method	Typical size range	Best part type	Main limit
Rigid tapping	M2 to M16	High hole count, through or blind holes	Tap reach and chip packing
Thread milling	M6 and larger	Large or near-shoulder threads, hard alloys	Longer cycle time per hole
Single-point turning	M3 and larger	Round parts needing concentric threads	Needs a lathe or mill-turn setup
Form tapping	M2 to M12	Aluminium, copper, mild steel	Higher spindle torque needed
Thread milling on mill-turn	M16 and larger	Parts with milled and turned features	Machine availability

FAQs

Common questions about threads for the CNC machining center

Why does my tap break on the reverse pass?

The most common cause is chip packing in a blind hole. A spiral-flute tap lifts chips out of the hole, but a deep hole still needs peck tapping or a larger pilot.

Check that the spindle reverses at the same speed and feed. A sudden speed change on the way out snaps small taps. Also confirm the programmed depth leaves at least one pitch of clearance at the bottom.

Can I thread mill a 6H internal thread without a gauge?

You can measure the pitch diameter with thread wires or a pitch micrometer, but a go/no-go gauge is faster on the shop floor.

The risk with thread milling is a wrong orbit radius. The thread looks correct and the crest is fine, but the pitch diameter is off. Gauge the first part of every run.

What pilot hole do I use for an M8 × 1.25 form tap?

Form tapping needs a larger pilot than cutting taps because the material is displaced, not removed. For M8 × 1.25 in aluminium, start near 7.4 mm and check with a gauge.

In 304 stainless, go slightly larger and use cutting oil. If the spindle load climbs, open the pilot by 0.05 mm and try again.

When is single-point turning better than tapping?

When the thread must stay concentric to a turned diameter. A milled or tapped thread sits wherever the hole sits, and hole position carries its own tolerance.

Turning also wins when the part is already on the lathe and adding a mill setup would double the workholding error.

How do I stop chatter when threading a long shaft?

Support the free end with a tailstock or steady rest once the length-to-diameter ratio passes about 4:1. Reduce the depth of the finishing pass to 0.05 mm.

A sharp insert and the correct infeed angle also help. If chatter persists, lower the spindle speed by 20% and take one spring pass.

Does plating change the thread fit?

Yes. Electroless nickel, zinc, and anodizing all add thickness to the flank. A coating of 0.01 mm per side closes the pitch diameter by roughly 0.02 mm.

Cut plated threads to the low side of the tolerance band, or mask the thread. Tell us about the finish when you request a quote so the allowance is built in.