Guide
A thread relief groove: what width, diameter and radius should a turned part call out at a shoulder?
A thread relief groove is a narrow turned groove, also called a thread undercut, cut just below the root of a thread where it meets a shoulder or the bottom of a bore, so that the threading tool can run out of the cut and the mating nut or screw can seat against the shoulder on full threads. It is defined by three numbers: the groove diameter, the groove width and the corner radius. For metric external threads those numbers are standardized by pitch in ISO 4755, and for inch threads they are usually derived from the thread’s minor diameter.
By Saola Manufacturing engineering team · Published · Updated
Many thread relief charts online are bare tables with no explanation of where the numbers come from. This guide gives the metric values by pitch, a matching inch table, the runout you get when there is no groove at all, the separate rules for internal relief, and a way to put the groove on a drawing that a lathe programmer and an inspector can both work from. How to write the thread itself is covered in the thread callout guide.
On this page
What does a thread relief groove do, and when does a turned part need one?
A thread relief groove gives the threading tool a place to stop and lets the mating part seat against the shoulder on complete threads. A turned part needs one whenever the full thread has to run right up to a shoulder, a flange or the bottom of a blind bore.
A single-point threading tool cannot stop dead at full depth. It has to either pull out of the cut over a short distance, which leaves a tapering incomplete thread called the runout or vanish thread, or finish inside an empty groove. Without a groove, the incomplete threads next to the shoulder stop a nut or a tapped part from screwing all the way down, so the joint clamps on the wrong surface or binds before it is tight. A groove removes that zone and keeps every thread up to the shoulder gaugeable.
The groove is not free. It removes cross-section exactly where a shaft steps down, and a groove with a sharp root concentrates stress at that step. That is why the standards give a corner radius for every pitch, and why the ISO metric undercut standard presents its grooves as recommended for cases where an undercut is actually needed, naming components such as plugs as the example (ISO 4755:1983). If the part is a highly loaded or fatigue-critical shaft, the choice between a groove and a controlled runout is a design decision, not a machining detail.
What width, diameter and radius does ISO 4755 give for a metric external thread relief?
Per ISO 4755, the groove diameter is the thread diameter minus a fixed amount per pitch, the maximum width is about three pitches, and the root radius is roughly half a pitch. Per ISO 4755, an M10 × 1.5 thread therefore gets a groove diameter of d minus 2.3 mm, a width between 2.5 and 4.5 mm and a radius of about 0.8 mm.
The table reproduces the standard’s values for the coarse pitches most turned parts use. The minimum width g1 is set by a transition angle of at least 30 degrees between the groove floor and the thread, and the maximum width g2 is measured from the shoulder face. The groove diameter carries an h12 tolerance up to and including 3 mm thread diameter and h13 above it, per ISO 4755:1983, which is a loose tolerance for a turned diameter. The German national standard DIN 76-1 publishes its own normal and short undercut forms for external threads (Form A and Form B, with a wider maximum width than ISO 4755), so a drawing should name the standard its values come from.
| Pitch P (mm) | Common coarse thread | Groove diameter dg (mm) | Width g1 min (mm) | Width g2 max (mm) | Radius r ≈ (mm) |
|---|---|---|---|---|---|
| 0.5 | M3 | d − 0.8 | 0.8 | 1.5 | 0.2 |
| 0.7 | M4 | d − 1.1 | 1.1 | 2.1 | 0.4 |
| 0.8 | M5 | d − 1.3 | 1.3 | 2.4 | 0.4 |
| 1 | M6 | d − 1.6 | 1.6 | 3 | 0.6 |
| 1.25 | M8 | d − 2 | 2 | 3.75 | 0.6 |
| 1.5 | M10 | d − 2.3 | 2.5 | 4.5 | 0.8 |
| 1.75 | M12 | d − 2.6 | 3 | 5.25 | 1 |
| 2 | M16 | d − 3 | 3.4 | 6 | 1 |
| 2.5 | M20 | d − 3.6 | 4.4 | 7.5 | 1.2 |
| 3 | M24 | d − 4.4 | 5.2 | 9 | 1.6 |
Two practical notes. First, the groove diameter in the table sits slightly below the minor diameter of the external thread, which is what lets the threading insert exit cleanly without touching the groove floor. Second, fine pitches use their own row: an M10 × 1 thread takes the pitch 1 values, not the M10 coarse values, because every dimension in the standard is keyed to pitch rather than to diameter.
What thread relief dimensions should an inch UNC thread use?
ASME B1.1 does not tabulate thread relief grooves, and there is no widely used inch counterpart to ISO 4755, so inch drawings normally set the relief diameter just below the thread’s minor diameter and size the width and radius from the pitch. Industry guidance from the precision machining trade puts the relief diameter at least 0.015 in below the minor diameter of an external thread.
The table applies that rule to common UNC sizes. The minor diameter used is the rounded-root UNR external minor from the basic Unified thread geometry in ASME B1.1, and the width and radius borrow the ISO proportions of about three pitches and half a pitch so that metric and inch parts in the same family behave alike. The 0.015 in clearance comes from the Precision Machined Products Association note on thread relief and chamfers, which also gives the internal rule used in the last column. Treat the values as a starting point to round to your drawing’s decimal convention, not as a standard table.
| Thread | Pitch P (in) | External relief diameter, max (in) | Width, max ≈ 3P (in) | Radius ≈ 0.5P (in) | Internal relief diameter, min (in) |
|---|---|---|---|---|---|
| 1/4-20 UNC | 0.0500 | 0.175 | 0.15 | 0.025 | 0.265 |
| 5/16-18 UNC | 0.0556 | 0.231 | 0.17 | 0.03 | 0.328 |
| 3/8-16 UNC | 0.0625 | 0.285 | 0.19 | 0.03 | 0.390 |
| 1/2-13 UNC | 0.0769 | 0.393 | 0.23 | 0.04 | 0.515 |
| 5/8-11 UNC | 0.0909 | 0.501 | 0.27 | 0.045 | 0.640 |
| 3/4-10 UNC | 0.1000 | 0.615 | 0.30 | 0.05 | 0.765 |
| 1-8 UNC | 0.1250 | 0.836 | 0.38 | 0.06 | 1.015 |
How long is the thread runout when there is no relief groove?
Per ISO 3508, the incomplete thread at the end of a fastener thread is normally up to about 2.5 pitches long, or about 1.25 pitches for the short form. On a fully threaded screw, the distance from the last full thread to the bearing face is normally up to about 3 pitches, with short and long forms at about 2 and 4 pitches.
Runout is what a part gets instead of a groove: the thread fades out as the tool retracts, and the length of that fade depends on the pitch, the retract move programmed on the lathe and the chamfer at the start of the thread. ISO 3508 standardizes the allowable runout and overrun for fasteners with ISO metric threads (ISO 3508:1976), and its pitch multiples are a useful benchmark for any turned thread that ends at a shoulder without a groove. For inch threads, the federal screw-thread handbook defines the effective thread as the complete threads plus those incomplete threads that are fully formed at the root, which leaves the vanish thread out of the useful length (NBS Handbook H28).
| Dimension | Form | Maximum, pitch multiple | M6 × 1 example (mm) |
|---|---|---|---|
| Run-out x (incomplete thread) | Normal | ≈ 2.5P | 2.5 |
| Run-out x (incomplete thread) | Short | ≈ 1.25P | 1.25 |
| Overrun a (last full thread to shoulder) | Normal | ≈ 3P | 3 |
| Overrun a (last full thread to shoulder) | Short | 2P | 2 |
| Overrun a (last full thread to shoulder) | Long | 4P | 4 |
The decision rule that follows from the table is simple. If the mating nut or part must clamp against the shoulder, the full-thread length has to reach closer than the overrun allows, so call out a groove. If the thread only has to engage over its middle, as on a stud that never bottoms, a controlled runout is cheaper and leaves more metal at the step. The PMPA note cited above gives a trade rule of thumb that external threads can usually be produced to within about one and a half threads of a shoulder without a groove, with the exact figure depending on pitch and on how well the material machines.
The chamfer at the start of the thread is the other end of the same budget. An entry chamfer down to the minor diameter protects the first thread from burrs, but every thread inside that chamfer is incomplete too, so the usable full-thread length is the threaded length minus the chamfer at one end and the runout or groove at the other. Specify both ends when engagement length is tight; the thread engagement guide shows how to size it.
How is an internal thread relief different from an external one?
An internal relief is cut above the thread’s major diameter instead of below its minor diameter, and it has to be wide enough for the tap chamfer or the boring-bar threading insert to finish inside it. As industry guidance, keep the internal relief diameter at least 0.015 in larger than the major diameter.
The diameter rule comes from the PMPA thread relief note, which also says internal threads can usually be tapped only to within about two and a half threads of a hole bottom when there is no relief. The width rule follows from the tool. A single-point internal threading tool needs about the same exit room as an external one, but a tap carries a chamfered lead whose first few teeth cut incomplete threads, so a tapped thread into a groove needs a groove at least as long as the tap’s chamfer plus some axial margin. DIN 76-1 gives separate normal and short internal undercut forms for metric threads in blind holes (DIN 76-1).
Internal grooves are also harder to make. They need an internal grooving tool that fits through the threaded bore, which limits them to holes large enough for a boring bar, and they cannot be inspected by eye. For small blind tapped holes the usual alternative is to drill deeper and accept incomplete threads at the bottom; how to state that depth is covered in the blind tapped hole depth guide.
How should a thread relief groove be dimensioned on a drawing, and what does it cost?
Either dimension the groove fully in an enlarged detail view, or reference the standard and its form in a note so the shop takes the values from the table. A standard groove on a turned part is usually a small cost, because it is one more pass with a grooving tool already in the turret.
An enlarged detail view, for example at 5:1, shows the groove diameter, the width from the shoulder face and
the corner radius, plus the transition angle to the thread if it matters. That suits inch drawings and any
groove that departs from a standard. A note works better for metric parts that follow the standard exactly,
for example THREAD UNDERCUT PER ISO 4755 next to the thread callout, or a DIN 76-1 form
designation where that standard is the house reference. Do not do both with conflicting values; a drawing
that says two different things about the same groove leaves the shop and the inspector to guess which one
governs.
Whichever method is used, tolerance the groove loosely. Groove diameter and width rarely need more than a general turned tolerance, and the radius is usually an approximate value. Over-tolerancing a relief groove adds inspection without adding function, while the thread pitch diameter and the shoulder face are where the tight tolerances belong.
On cost, the comparison is groove versus runout, not groove versus nothing. On a CNC lathe the groove is cut in the same setup as the thread, and it can make threading itself simpler because the insert does not have to retract under a controlled pull-out. Where cost does climb is on internal grooves in small bores, grooves with tight radius or width tolerances, and grooves on parts that are otherwise milled rather than turned. When we review a drawing for CNC turning, we check whether the groove diameter clears the minor diameter, whether the radius suits a standard grooving insert, and whether a thread on a milled part such as a manifold port would need a relief that a CNC milling setup can reach. If the relief is optional, say so on the RFQ so the quote can offer both versions. A drawing can be sent through the quote form.
Frequently asked
Is a thread relief the same as a thread undercut?
Yes. Thread relief, thread undercut, relief groove and thread runout groove all describe the same feature. ISO 4755 uses “thread undercut”, DIN 76-1 uses “Gewindefreistich”, and many inch drawings simply say “relief”.
Is thread runout the same thing as a relief groove?
No. Runout is the incomplete, tapering thread left when the tool retracts without a groove; a relief groove replaces that zone with a plain turned diameter. ISO 3508 limits how long the runout may be, while ISO 4755 sets the groove that removes it.
Can I use a DIN 509 undercut for a thread?
Not as a substitute. DIN 509 undercuts are sized for clearance at ground and turned shaft shoulders, not for threading tool runout, so their depth and width do not follow thread pitch. Use the thread undercut standard for threads, and see the fillet vs chamfer guide for edge breaks at the same step.
Does a relief groove weaken a bolt or shaft?
It can. The groove floor is smaller than the thread minor diameter, so it becomes the smallest section, and a sharp root adds a stress raiser. Keep the standard radius, and for fatigue-loaded parts compare the groove floor area with the thread stress area before choosing a groove over runout.
Do rolled threads need a relief groove?
Usually not in the same way. Thread rolling dies leave their own runout and cannot form threads right up to a shoulder, so rolled parts are normally specified with a runout allowance per the fastener standard rather than a cut groove. Ask the supplier which process they plan before fixing the groove.
Sources
- ISO 4755, Fasteners: Thread undercuts for external metric ISO threads, International Organization for Standardization, first edition 1983
- ISO 3508, Thread run-outs for fasteners with thread in accordance with ISO 261 and ISO 262, International Organization for Standardization, 1976
- DIN 76-1, Fasteners: Thread run-outs and thread undercuts, Part 1: For ISO metric threads in accordance with DIN 13-1, DIN Media, 2025 edition (supersedes the 2016-08 edition)
- ASME B1.1, Unified Inch Screw Threads, ASME, 2024 edition
- Screw-Thread Standards for Federal Services, Handbook H28, Part I, National Bureau of Standards, 1969
- Thread Relief and Chamfers, Precision Machined Products Association, accessed 2026