Guide
When is single point threading the right way to make a thread, compared with tapping, rolling or thread milling?
In short, single point threading is cutting a thread on a lathe with one profiled insert that makes a series of passes, with the feed per revolution locked to the thread pitch. It is the usual choice for external threads on turned parts, for large or non-standard pitches, for tapered pipe threads and for Acme-type profiles; tapping wins for small internal threads, rolling for high-volume external threads that need fatigue strength, and thread milling for threads on non-rotating parts or close to a shoulder.
By Saola Manufacturing engineering team · Published · Updated
Two neighboring choices have their own guides: thread milling vs tapping for holes on milled parts, and rolled vs cut threads for custom screws. This page puts single point threading next to all three and explains when the lathe should cut the thread.
On this page
How does single point threading work?
The lathe synchronizes the tool feed with spindle rotation so the tool advances one pitch per revolution, and the insert cuts the thread depth in several passes. Each pass follows the same helix, so the thread builds up gradually.
Sandvik Coromant's thread turning guidance states the basic rule, that the feed rate must equal the thread pitch, and that the tool makes a number of passes with an adequate depth of cut on each (Sandvik Coromant, thread turning). Because the tool works around the part's own axis, the thread is made in the same setup as the other turned diameters, which keeps it concentric with them.
The way the tool moves into the cut matters. Sandvik describes radial infeed as common and the only option on many non-CNC lathes, suited to fine pitches but prone to stiff chips and vibration on large pitches; modified flank infeed as the first-choice method, with the best chip control and tool life; and incremental infeed as the choice for very coarse profiles, at the cost of harder chip control and a special program (Sandvik Coromant, infeed methods). You rarely specify this, but it explains why a supplier may quote a coarse thread in a tough material with a longer cycle.
How do the four threading methods compare?
They differ mainly in which features they can reach, which profiles they make, how they behave near a shoulder, and how fast they are. The table compares them on the points that usually decide the choice on a drawing.
Sandvik summarizes the cutting methods this way: thread turning for rotating parts threaded about their own axis, covering the largest number of thread profiles; thread milling for non-rotating parts, off-center threads and large workpieces, with low cutting forces and no need for a relief groove near a shoulder; and tapping as a productive, economical method especially for smaller threads (Sandvik Coromant, threading overview). Rolling is a forming process rather than cutting, covered in the rolled-thread guide.
| Point | Single point threading | Tapping | Thread milling | Thread rolling |
|---|---|---|---|---|
| Best feature | External threads on turned parts; large internal threads | Small and medium internal threads | Internal or external threads on milled or non-rotating parts | External threads on pins, screws and studs |
| Profiles | Widest range: UN, metric, NPT taper, Acme, buttress, special | Standard profiles that taps exist for | Most profiles; one tool can cover several diameters of the same pitch | Standard and special forms with dedicated dies |
| Near a shoulder or blind bottom | Needs a relief groove or runout | Needs room for the tap chamfer below the full thread | Can thread close to a shoulder without a relief groove | Needs runout for the die |
| Concentric with other diameters | Yes, made in the same setup | Follows the drilled hole | Set by the machine path | Follows the blank |
| Cycle time per thread | Several passes | Fastest for small holes | Moderate | Fast once set up |
| Typical volume | Prototypes to production | All volumes | All volumes | Production; tooling cost up front |
| Acceptance | Go/no-go gauges to the stated class | Go/no-go gauges | Go/no-go gauges | Go/no-go gauges, plus any fatigue or lap requirement |
When should a turned part have a single-point thread?
Choose it when the thread is external and on the part's axis, when the size or pitch has no standard tap or die you would want to buy, or when the thread must run true to other turned diameters. It is also the normal way to cut tapered pipe threads and Acme or trapezoidal threads on a lathe.
Typical cases are threaded ends on shafts and fittings, threaded bodies on valves and adapters, large internal threads in turned housings, and lead-screw style Acme threads. For pipe threads, the taper is cut by the same synchronized motion with the cross-slide moving at the same time; the thread is then gauged to the taper standard, such as ASME B1.20.1 for NPT. The NPT thread chart and Acme vs trapezoidal guide cover those profiles.
Single point threading is a poor fit for small internal threads, where a tap is faster and the boring bar would be too slender, and for very high volumes of plain external threads, where rolling is faster and gives a stronger root. It is also slower than tapping because of the multiple passes, so on a part with many small tapped holes, those holes are almost always tapped.
What does a single-point thread need from the drawing?
Give the thread designation and class, the full-thread length, and either a relief groove or an acceptable runout length at a shoulder. Do not name the method unless function requires it.
ASME B1.1 specifies the thread form, series, class, allowance, tolerance and designation for unified inch threads (ASME B1.1-2024), so a callout such as 3/4-16 UNF-2A already defines the result. Adding SINGLE POINT on the drawing only restricts the supplier; the exception is when a rolled thread is required, or forbidden, for fatigue or material reasons.
The shoulder is where single-point threads cause the most queries. The tool needs space to withdraw at the end of each pass, so the drawing should show a thread relief groove or state how many incomplete threads are allowed before the shoulder. The thread relief groove guide gives the usual groove shapes, and the thread callout guide covers the designation itself.
How is a single-point thread inspected?
With go/no-go thread ring or plug gauges to the stated class, and for critical threads a pitch diameter measurement. The method used to make the thread does not change the acceptance test.
ASME B1.2 gives the specifications and dimensions for the gauges and measuring equipment used on unified inch screw threads and describes the purpose of each gauge (ASME B1.2-2025). In practice a go ring or plug that assembles and a no-go that does not enter more than allowed is the routine acceptance; the go/no-go gauge guide explains how to read the result.
Watch two features that are specific to single-point threads: the crest of the first thread, which should be chamfered so the gauge and the mating part start cleanly, and the torn or ragged flanks that can appear in soft, gummy materials when the infeed is wrong. If either matters, add a chamfer callout and a visual requirement for flank condition. For a deeper check, the pitch diameter guide covers wire measurement.
How are threads handled on a Saola order?
Threads are cut at the lead plant as part of turning and milling, the method for each thread is chosen at drawing review, and threads are gauged with go/no-go gauges. Pipe threads such as NPT are gauged to ASME B1.20.1.
The CNC turning page covers small-diameter bar and tube parts on conventional CNC lathes; external threads on those parts are made in the turning setup, and holes on milled parts are covered on the CNC milling page. If your drawing requires rolled threads, say so in the RFQ so that process is confirmed at drawing review before quoting.
Send the drawing for a quote with every thread callout complete, including class, length and the relief at any shoulder.
Frequently asked
Is a single-point thread weaker than a rolled thread?
In static strength the difference is usually small; in fatigue a rolled thread is typically better because the root is cold-worked and the grain flows around it. If fatigue matters, specify rolled threads; the rolled vs cut guide covers when that is worth it.
Can single point threading make left-hand threads?
Yes. The lathe reverses the tool direction or uses a left-hand insert. Mark LH in the thread designation so the gauge and the program match.
Why does my supplier ask for a relief groove?
Because the tool must stop and withdraw at the end of every pass. Without a groove, the last threads near a shoulder are incomplete, and the drawing needs to say how many incomplete threads are acceptable.
Can internal threads be single-pointed?
Yes, with a threading boring bar, as long as the bore is large enough for a rigid bar. Small internal threads are normally tapped instead.
Does the method change the thread class I should specify?
No. Specify the class the function needs, such as 2A/2B or 3A/3B, and the supplier picks a method that meets it. The thread class guide explains the difference.
Sources
- Threading: thread turning, thread milling, tapping and thread whirling (overview), Sandvik Coromant technical guidance, accessed November 2026
- Thread turning, Sandvik Coromant technical guidance, accessed November 2026
- How to choose infeed method in thread turning operations, Sandvik Coromant technical guidance, accessed November 2026
- ASME B1.1-2024, Unified Inch Screw Threads (UN, UNR and UNJ Thread Forms), ASME, 2024
- ASME B1.2-2025, Gages and Gaging for Unified Inch Screw Threads, ASME, 2025