A Complete Understanding of Thread Processing Methods
This guide covers how internal and external threads are cut, rolled and ground on CNC machines. It is for design engineers and buyers who must pick a method, set a tolerance and avoid scrap. After reading, you can match a thread callout to a process and an inspection plan.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
What matters before you choose a method
How thread processing methods divide by function
Threads split into two jobs. Connection threads hold parts together: bolts, sensor bosses, hydraulic ports, filter housings. Here the priorities are fit class, interchangeability and cycle time. Transmission threads move a load: lead screws, ball screw nuts, worm gears, adjusting screws. Here the priorities are lead accuracy, flank finish and long-term wear.
That split decides the process before any drawing detail is read. A M6 threaded hole in an aluminum bracket is a tapping job. A 40 mm × 6 mm trapezoidal screw 800 mm long is a turning and grinding job. Treating them as the same task is where most quoting errors start.
A second variable is thread position. External threads on a shaft can be cut on a lathe, rolled between dies or milled with a thread mill. Internal threads in a blind hole are far more restricted. If the hole is deeper than about 2.5 × diameter, tap breakage risk climbs and thread milling becomes the safer route.
Finally, material hardness sets the ceiling. Above roughly 35 HRC, cutting tools wear fast and rolled threads are no longer practical because the material will not flow. That is the point where grinding takes over for external threads.
Cutting methods: turning, milling and tapping
Single-point turning uses a 60° or 55° insert fed along the axis while the spindle rotates. The machine's feed chain must stay synchronized to the spindle, so the thread lead is a function of the CNC interpolation, not of the operator. For a complete understanding of thread processing methods, this is the base case: it is flexible, needs no special tooling per pitch and suits one-offs and prototypes.
Thread milling interpolates a smaller tool around the bore on a helical path. It works on holes that are too large or too awkward for a tap, and the same tool handles right-hand and left-hand threads. Because the tool is small, cutting force is low, which helps on thin-walled parts and on titanium. On our 5-axis centers we use it for port threads and for any hole where a broken tap would scrap the part.
Tapping drives a shaped tool into a drilled hole, cutting or forming the thread in one pass. It is the fastest method for small and medium internal threads. Cutting taps need a drilled hole near the nominal minor diameter; forming taps need a larger pilot hole because they displace material rather than remove it. Forming taps produce no chips, which matters in blind holes and in medical parts where a trapped chip is a reject.
The usual failure is a snapped tap in a deep blind hole. Use spiral-flute taps for blind holes so chips come out the top, keep thread depth to about 2 × diameter plus two pitches, and run a peck cycle with full retract on anything past 2.5 × diameter.
Rolling and grinding for strength and accuracy
Thread rolling presses a blank between two or three dies. The material flows cold into the die form instead of being cut away, so the grain runs continuously through the root. On steel studs and on aluminum fasteners this raises fatigue resistance and leaves a smoother flank, often Ra 0.4–0.8 μm straight off the machine. Blank diameter must be set correctly, usually close to the pitch diameter for the given class, or the crest will be underfilled or oversized.
Rolling has hard limits. It only works on ductile material, it needs a diameter large enough to survive the forming pressure, and it cannot produce threads up to a shoulder because the dies need run-out room. It also does not fix an out-of-round blank. If the pre-rolled diameter is turned poorly, the rolled thread inherits the error.
Thread grinding uses a profiled wheel on an external grinder. A single-rib wheel dresses the full form and produces class 5–6 accuracy with flank finish in the Ra 0.2–0.8 μm range. This is the process for hardened shafts, gauge-quality threads and worm shafts that must hold lead over a long length. It is slow and it needs a dedicated machine, so it is reserved for the parts that genuinely need it.
Between rolling and grinding there is a cost gap of several times on the same part. Choose rolling when strength and surface finish matter but class 6H/6g is enough. Choose grinding when the drawing calls for lead accuracy measured in micrometers over hundreds of millimeters.
Material behavior changes the choice
Aluminum 6061 and 6082 tap and roll easily but are prone to galling, so use a lubricant and keep cutting speed high enough to avoid built-up edge. Thin aluminum walls distort under forming taps. If the wall is under about 1.5 mm, cut the thread rather than form it.
Stainless 304 and 316 work-harden quickly. A tap that rubs instead of cutting will harden the surface and then break. Use a sharp tap, a slow speed around 8–15 m/min and never reverse mid-hole to clear chips without a full retract. 303 machines far better because of its sulfur content, but it is not always acceptable for corrosion service.
Titanium Ti-6Al-4V and Inconel are the difficult cases. Tapping is risky above M6, so thread milling with a rigid small tool and generous coolant is the safer route. Heat stays in the tool, so keep the radial engagement low and the feed per tooth steady.
Plastics like POM, PC and PEEK need coarse threads and low spindle speed. Rolled threads in plastic can split the wall, and a tight fit class will seize. Allow clearance and specify a looser class than you would for metal.
How to pick and run a thread process
- 11. Classify the thread by functionMark the callout as connection or transmission. Connection threads: aim for 6H/6g unless the drawing says otherwise. Transmission threads: note lead accuracy and length, because these drive the machine choice.
- 22. Check hardness and ductilityBelow about 35 HRC and ductile, rolling is on the table. Above 35 HRC, plan for grinding on external threads and thread milling or EDM on internal ones. Do not schedule a tap into hardened steel.
- 33. Match the method to positionThrough holes and shallow blind holes: tapping. Deep blind holes past 2.5 × diameter: thread milling. External, high volume, no shoulder: rolling. External, tight lead: grinding.
- 44. Set the pilot hole from the tap chartCutting taps use the minor diameter; forming taps use a larger hole, roughly the pitch diameter minus a small allowance. A 0.05 mm error in the pilot hole shifts the thread class and can cause tap breakage at the bottom.
- 55. Fix speed and feed before the first partTypical ranges: aluminum 60–120 m/min, carbon steel 15–30 m/min, stainless 8–15 m/min, titanium 5–12 m/min. Feed equals pitch × spindle speed. Rigid tapping on a synchronized spindle removes the need for a floating holder.
- 66. Control the run-outTap and thread mill run-out should stay under 0.02 mm, ideally 0.01 mm. A holder with more run-out will cut an oversized thread on one flank and a tight thread on the other.
- 77. Inspect pitch diameter, not major diameterUse a thread micrometer or a three-wire set. Calipers on the major diameter tell you almost nothing about fit. Check pitch diameter, then check the gauge goes on by hand.
- 88. Deburr and verify before shippingBreak the start and end of every thread. A burr at the entry changes the effective class and will fail a go/no-go check. We inspect 100% of threaded features before shipment and can supply reports on request.
Thread processing methods compared
Typical ranges for steel and aluminum parts; exact values depend on material and setup.
| Method | Best for | Typical accuracy | Main limit |
|---|---|---|---|
| Tapping | Internal threads up to about M30 | Class 6H, Ra 1.6–3.2 μm | Taps break in deep blind holes |
| Single-point turning | External threads, one-offs, prototypes | Class 6g, Ra 1.6–3.2 μm | Slow on long production runs |
| Thread milling | Large or awkward internal threads | Class 6H, Ra 0.8–1.6 μm | Longer cycle than tapping |
| Thread rolling | High-volume studs and fasteners | Class 6g, Ra 0.4–0.8 μm | No thread up to a shoulder |
| Thread grinding | Hardened and gauge-quality threads | Class 5–6, Ra 0.2–0.8 μm | Slow and machine-specific |
Pick the method from the function, not the habit
If the thread only holds a fastener, tap it or roll it and spend your tolerance budget elsewhere. If it transmits motion or must hold lead over length, plan for turning and grinding from the start.
Thread processing questions engineers ask
Why does my tapped hole gauge tight on the first few parts?
The usual cause is thermal growth. The tap and the part both heat up during a run, so the first holes cut slightly small and later holes drift. Measure the first part cold, then re-check after ten parts.
Run-out in the holder is the second cause. Above 0.02 mm the thread flanks become asymmetric and the go gauge drags.
Can rolled threads replace cut threads on a drawing?
Often yes, and they are stronger. But the blank diameter and the run-out at the thread end both change, so the drawing has to allow a slightly larger minor diameter and some relief at the shoulder.
If the part is hardened after threading, rolling is not an option. Roll before heat treatment or grind after it.
What thread depth should I allow in a blind hole?
Allow the full thread depth plus two pitches for the tap lead-in, plus clearance at the bottom. For an M6 × 1 hole with 12 mm of full thread, plan a drilled depth of about 16–17 mm.
If the design cannot give that room, switch to thread milling. A thread mill needs less bottom clearance than a tap.
When is thread milling cheaper than tapping?
Rarely on small holes in high volume. Thread milling wins when the hole is large, when the material is difficult, or when a broken tap would scrap an expensive part.
It also wins when one tool must cover several thread sizes, because a single thread mill can interpolate different diameters.
How do you inspect thread accuracy without gauges?
Use a three-wire set with a micrometer to measure pitch diameter, or a thread micrometer with the correct anvil. Both give a number you can record against the drawing.
Optical comparators work for form and flank angle but not for fit. For production, a go/no-go gauge is still the fastest check.
Does thread grinding change the material properties?
It removes a small amount of material and can leave grinding burn if the wheel is dull or the coolant is poor. On hardened steel, watch for a light temper color on the flank.
A dressed wheel and steady coolant flow keep the surface clean and hold the Ra 0.2–0.8 μm range.
Send your thread drawing for a process review
We review the callout, the material and the depth, and come back with a method, a tolerance and a price.
12-hour quoteFree DFM analysisNo minimum order quantity100% inspection
More CNC process notes
We publish setup notes, tooling trials and inspection data from the factory floor.
