Thread Fit Calculator
Thread
Defaults are the commercial standard M12 × 1.75 with a 6H/6g fit. Basic pitch diameter d2 = d − 0.6495·P; basic minor diameter d1 = d − 1.0825·P.
Result — limits in mm
Allowance (es / EI)34 µm
External major d11.966 – 11.707
External pitch d210.829 – 10.681
Internal pitch D210.863 – 11.059
Internal minor D110.106 – 10.446
Min clearance (pitch)0.034 mm
Max clearance (pitch)0.378 mm
FitClearance fit
Tolerances Td2 / TD2 / Td / TD1148 / 196 / 259 / 340 µm
Values are computed from the ISO 965-1 tolerance formulae. The published ISO 965-2 limit tables may differ by a few micrometres due to the standard's rounding; check a handbook table when the number feeds a gauge design.
What is Thread Fit Calculator
Thread Fit Calculator works out the limit dimensions and the resulting fit of an ISO metric screw thread pair from its tolerance classes. You enter the nominal diameter, the pitch, the internal class such as 6H and the external class such as 6g, and the tool computes the basic pitch and minor diameters, the allowance, the tolerance widths, and the full set of limit diameters: external major and pitch, internal pitch and minor, plus the minimum and maximum pitch-diameter clearance of the fit.
The arithmetic follows ISO 965-1: the basic pitch diameter is the nominal minus 0.6495 times the pitch, the basic minor diameter is the nominal minus 1.0825 times the pitch, grade-six tolerance widths come from the standard's formulae in micrometres — 90 times pitch to the 0.4 power times the diameter-range mean to the 0.1 for the pitch diameter, 180 times pitch to the two-thirds minus 3.15 over the square root of pitch for the external major, and 230 times pitch to the 0.7 for the internal minor — scaled by the standard grade multipliers. Fundamental deviations follow the position letters: h and H at zero, g per the standard's table, and f and e from the 30-plus-11-pitch and 50-plus-11-pitch formulae.
How to Use Thread Fit Calculator
- Step 1: Enter the nominal diameter in millimetres — 12 for an M12 thread.
- Step 2: Pick the Pitch from the standard series, from 0.8 to 3 millimetres. The coarse pitch for M12 is 1.75.
- Step 3: Pick the internal class — 4H through 8H, with 6H the commercial default for tapped holes.
- Step 4: Pick the external class — grades 4 through 8 in positions h, g, f and e, with 6g the commercial default for bolts.
- Step 5: Read the result: the allowance, the external major and pitch limits, the internal pitch and minor limits, and the minimum and maximum clearance of the fit.
The default combination — M12 by 1.75 with a 6H internal and 6g external class — is the most common commercial fit in the world: an uncoated metric bolt in a tapped hole. The fit row reports whether the pair is a clearance fit, and the two clearance rows give the pitch-diameter play at best and worst material condition.
Why Use Thread Fit Calculator
Thread fits decide whether a bolt drops into a tapped hole, whether a coating still assembles after plating, and whether a thread-milling cutter can hold the tolerance a drawing calls out. The default 6H/6g is right for general commercial use, but plating, heat treatment and precision work all move the classes — 6e and 6f exist to absorb coating thickness, and grades 4 and 5 exist for gauge-quality threads.
The tool is equally useful reading a drawing backwards: a callout such as M16 by 2, 6H/6g, gives you the exact material limits the machinist and the inspection department are working to, and the clearance rows tell you how loose the pair actually is — the number behind every thread-fit judgement you will make on the shop floor.
Privacy & Security
This tool runs entirely in your browser — no data ever leaves your device. There is no server round-trip, no upload, no logging, and no account required. Your input is processed locally using client-side JavaScript and is never stored, transmitted, or accessible to anyone else. When you close the tab, everything disappears.
Frequently Asked Questions
What does 6H/6g actually mean?
Two tolerance classes separated by a slash: 6H for the internal thread and 6g for the external. The 6 is the tolerance grade — the width of the permitted variation — and the letter is the position, the allowance side. H and h sit at the basic profile with zero allowance, and g, f and e move the external thread smaller to guarantee clearance. For M12 by 1.75, the g position carries a 34 micrometre allowance, so the external pitch diameter tops out at 10.829 millimetres against a basic value of 10.863.
Why is the external pitch diameter maximum smaller than the basic value?
Because the position letter g applies a fundamental deviation that shrinks the external thread to guarantee clearance against an H internal thread. For M12 by 1.75 the allowance is 34 micrometres, so the pitch diameter can never exceed 10.829 millimetres even at maximum material condition. The internal thread starts exactly at the basic 10.863, which is what guarantees the pair always has at least a small clearance rather than an interference fit.
What is the difference between 6g and 6h?
Only the allowance. Both use grade 6 widths, but h has a zero fundamental deviation — the thread can reach the full basic size — while g sits below it. The h position is used for precision fits and maximum strength, and g is the general-purpose commercial position that gives plating and assembly clearance. Everything else about the two classes computes identically.
How do I allow for plating on a thread?
Pick an external position with a larger allowance than g: f and e exist exactly for coatings. A typical zinc plating of 5 to 15 micrometres fits a 6f or 6e thread, and thicker hot-dip galvanizing needs the special allowances of ISO 965-4. The rule is that tolerances apply before coating, and the plated thread must still stay inside the basic profile after coating — which is what the extra allowance buys.
Why might the numbers differ slightly from my handbook table?
The tool computes the limits from the ISO 965-1 tolerance formulae directly, while printed handbooks and ISO 965-2 publish the rounded results of those formulae. The differences are a few micrometres at most. If the number is feeding a gauge design or a thread-limit inspection, cross-check the computed limits against a published table for the exact size and class first.