Thread Root Relief Calculator — Guide

The problem this solves

Thread tables give pitch and nominal diameter. They rarely give the major, minor and pitch diameters directly — and they assume you're cutting with an insert ground to the thread standard's own root radius.

Most general-purpose threading inserts aren't. A "sharp" generic nose radius is usually smaller than the radius the standard intends. If you feed that insert in until the flanks land in the right place (correct pitch diameter, correct fit), it will also cut deeper into the root than the standard calls for — a sharper, weaker notch at the base of the thread than was ever intended.

This calculator works out exactly how much deeper that is, and gives you a way to avoid it: cutting the same depth in two slightly offset passes instead of one, so the root ends up at the correct depth without ever cutting past it.

Using the calculator

1. Choose the thread family — ISO Metric / UN (60° included) or Whitworth (55° included). This sets the flank angle and the standard's default root radius.
2. Enter the pitch and major diameter. Pitch can be typed directly in mm, or as TPI for imperial threads — the "enter as TPI" link converts it for you.
3. Check the ideal root radius field. It auto-fills from the thread standard (0.144 × P for ISO/UN, the Whitworth standard radius for BSW/BSF) but can be overridden if you're working to a specific drawing callout.
4. Enter your insert's actual nose radius. This is on the insert manufacturer's data sheet — don't guess it. If you don't have a spec sheet, measure it under a toolmaker's microscope or against radius gauges.
5. Read the depth comparison. If the actual radius is smaller than ideal, the calculator flags how much deeper a naive single pass would cut, and the next section gives you the fix.

Programming the two passes

Both passes are cut to the same X depth — the depth the ideal-radius tool would reach. Only the starting angle differs between them, which shifts the cut a fraction of a millimetre along the thread axis. On a Fanuc-style control this is the Q parameter of the G76 threading cycle (starting angle, in 0.001° units).

Worked example for M10×1.5 with a 0.1mm insert nose radius (the calculator's default values):

Checking the result

This calculation assumes a straight radial infeed and treats the thread as a 2D cross-section — it doesn't account for helix/lead angle, insert deflection, or how your particular insert actually seats and wears. Treat the output as a strong starting point, not a guarantee.

1. Cut both passes to the calculated depth.
2. Check fit against a thread ring gauge or a witness nut on the flanks.
3. If it's tight, sneak in another 0.01–0.02mm on both passes and recheck — don't jump straight back to a single deeper pass, or you'll reintroduce the over-cut root this method exists to avoid.

Notes & FAQ

What if my insert's nose radius is larger than the ideal radius?

The calculator will flag this and the two-pass method doesn't apply — an oversized radius leaves the root shallower than the design profile, not deeper, so there's nothing to relieve. Cut a single pass to the ideal depth.

Does the offset between the two passes affect where the thread sits axially?

Very slightly — by roughly half the calculated separation, if you simply offset the second pass from the first. The calculator also gives a "centred" version (split equally either side of the nominal start) that keeps the pitch line exactly on the programmed centreline, for cases where that matters. For most threads taking a nut, it doesn't.

Why not just use a properly radiused insert instead?

You should, when one's available for the size and form you need. This tool is for the common shop-floor case: a generic threading insert that doesn't have the exact radius the standard calls for, and no immediate access to one that does.