DatumCalc

CNC / machinist calculator

Thread Dimension Calculator (Pitch and Minor Diameter)

Get the basic dimensions of a 60-degree thread from its major diameter and pitch. Enter an inch thread by its threads per inch or a metric thread by its pitch in millimetres and this calculator returns the pitch diameter, the basic minor diameter and the single-point cutting depth. These are the numbers behind a thread callout, useful for inspection, single-point turning and modeling, and they sit alongside the tap drill tool, which answers the separate practical drilling question.

Pick a class to see min/max limit dimensions.
Pitch diameter
-
Basic minor diameter
-
Single-point cut depth
-

Class limits per ISO 965-1:1998 (metric 6g / 6h / 6H) and ASME B1.1-2003 (unified 1A / 2A / 3A / 1B / 2B / 3B), reproduced from the standards' formulas and pinned to their published tables. A mid-limit is the middle of a tolerance zone, the value CAD systems such as Fusion 360 dimension a toleranced thread to. The internal major diameter has no tabulated maximum, so its mid-limit uses the theoretical sharp-V apex as the max: major mid = major min + H / 8, where H is the 60-degree fundamental thread height. The external minor diameter depends on the root form the tool cuts, so the flat-root and rounded-root (UNR / radiused) maxima are shown along with the rounded-root minimum and the minimum and basic root radius. Reference values; verify against your gauge or print.

Saved setups

Saved in this browser only. Export to move setups between machines.

How it works

A 60-degree thread is defined by its major diameter and its pitch, and the rest of the basic profile follows from the geometry. The pitch diameter, the effective diameter where the thread thickness equals the groove width, is the major diameter minus 0.6495 times the pitch. The basic minor diameter, the bottom of the internal thread, is the major diameter minus 1.0825 times the pitch.

These basic dimensions describe the ideal profile of the standard, ISO 724 for metric and the Unified standard for inch. They are not the same as the tap drill size, which deliberately leaves a partial thread, around seventy-five percent, to cut tapping torque. So the minor diameter here is the basic full-thread minor, while the tap drill tool gives the practical hole to drill.

For single-point turning of an external thread, the cutting depth is about 0.6134 times the pitch, the standard infeed for a 60-degree form. The single-point threading tool turns that total depth into a pass-by-pass infeed schedule.

Real threads are made to a tolerance class, not to the basic profile. Pick a class and this calculator also returns the limit dimensions: for metric threads the ISO 965 classes 6g and 6h (external) and 6H (internal), and for unified inch threads the ASME B1.1 classes 1A, 2A and 3A (external) and 1B, 2B and 3B (internal). External classes take their tolerance downward from the basic size (classes 1A, 2A and 6g also subtract an allowance for plating and guaranteed clearance), while internal classes grow upward from it. The pitch diameter limits are what GO and NO-GO thread gauges actually check, and the reported mid-limit, the middle of that tolerance zone, is the single value CAD systems like Fusion 360 dimension a toleranced thread to. The tolerances come from the standards' formulas, and where a printed table in the standard differs from formula rounding, the printed value is used, because that is what gauges are made to.

pitch dia = major - 0.6495 × pitch | basic minor = major - 1.0825 × pitch | single-point depth ~ 0.6134 × pitch

Worked example

A 1/4-20 thread (major 0.25 in, pitch 0.05 in) has a pitch diameter of 0.25 - 0.6495 x 0.05 = 0.2175 in, and a basic minor near 0.196 in.

Hat tip

The tolerance-class feature was prompted by, and is cross-validated against, threadmill by Andrew Downing (MIT-licensed source). DatumCalc's engine is independently implemented from ISO 965-1:1998 and ASME B1.1-2003 and agrees with his on all 274 cross-checked limit values, plus the external minor diameter and root-radius limits added at his suggestion.

Frequently asked questions

What is the pitch diameter of a thread?

The pitch diameter is the effective diameter where the width of the thread ridge equals the width of the groove. For a 60-degree thread it is the major diameter minus 0.6495 times the pitch, and it is the diameter that governs fit.

How is the minor diameter different from the tap drill?

The basic minor diameter is the bottom of a full standard thread, the major diameter minus 1.0825 times the pitch. The tap drill is deliberately a little larger to leave about a seventy-five percent thread, which cuts tapping torque, so the two numbers differ.

What is the cutting depth for single-point threading?

For a 60-degree external thread the standard single-point cutting depth is about 0.6134 times the pitch. The single-point threading tool splits that total depth into decreasing passes so each pass removes a similar chip area.

Do these formulas work for metric threads?

Yes. The 60-degree geometry is the same for ISO metric and Unified inch threads, so the factors 0.6495 and 1.0825 apply to both. Just enter the pitch in millimetres for metric or as threads per inch for inch threads.

What is the pitch diameter used for?

Pitch diameter is the dimension that actually controls how a thread fits and is what thread gauges and the three-wire method measure. Major and minor diameters set clearance, but the pitch diameter sets the class of fit.

What do thread tolerance classes like 6g or 2A mean?

A class packages a tolerance size and its position relative to the basic profile. Metric 6g is the default external bolt class with a small allowance below basic, 6h has no allowance, and 6H is the default internal nut class. Unified 2A/2B are the general-purpose external/internal classes with an allowance on 2A, 3A/3B are tighter classes with no allowance for critical fits, and 1A/1B are loose classes, half again wider than 2A/2B, for dirty or plated assemblies that must still go together.

What is the mid-limit pitch diameter?

It is the middle of the pitch diameter tolerance zone, halfway between the min and max limits. CAD systems such as Fusion 360 dimension a toleranced thread to this value, and it makes a sensible single machining target: aim at the middle and normal process variation stays inside the limits.

Why does an external thread class show no minor diameter limits?

For external threads the thread root is controlled by the form of the cutting tool rather than by a toleranced diameter pair, so the standards specify a minimum root radius instead of minor limits. Internal classes do get minor diameter limits, and those are what the tap drill and go plug gauge relate to.

Related calculators

Coverage

Implements ISO 965-1:2026 (metric) + ASME B1.1-2003 (unified) tolerance classes: 6g, 6h, 6H, 1A, 2A, 3A, 1B, 2B, 3B, external minor diameter and root-radius limits (ISO: flat-root max, rounded-root max/min, root radius min/basic; Unified: UNR rounded-root max, root radius min/basic). Deliberately not offered yet:

Sources

Every formula on this page is shown and sourced. See how we verify.

These calculators are for planning and as a starting point. Recommended speeds and feeds are published starting values that vary with your specific tool, coating, machine rigidity, workholding and coolant. Always start conservative, listen to the cut, and follow your tool maker data sheet.