Clearance Hole Calculator

Clearance Hole Calculator results give the hole a metric or inch bolt needs at close, normal or loose fit, plus the hole tolerance, how far every hole can wander and the tap drill.

Clearance Hole Calculator for Metric and Inch Bolts

A clearance hole is the plain hole a bolt or screw passes through without threading into it. Drill it too small and the parts will not go together, and drill it too big and the head loses bearing while the parts can shift.

Machinists, fabricators and designers use the result to pick a drill, write the hole callout on a drawing, and set how accurately the hole pattern must be located. Makers and DIY builders use it to find which drill to grab for an M6 or 1/4 inch bolt.

The Clearance Hole Calculator reads the standard tables for metric and inch fasteners. Beyond the hole size, it shows the largest hole the tolerance allows and the position tolerance for the pattern. It also gives the tap drill if the mating part is threaded, plus the nut and washer sizes around the hole.

Bolt Standard, Size, Fit Class and Pitch

In the Clearance Hole Calculator, pick Metric (ISO 273) for M1.6 to M36 or Inch (ASME B18.2.8) for #0 to 1-1/2 inch, then the bolt size and fit class. Close fit holds parts in place most accurately, normal fit is the everyday choice, and loose fit absorbs misalignment.

Thread pitch only changes the tap drill card. An M8 coarse and an M8 fine bolt share the same 8 mm major diameter, so both take the same clearance hole.

The Hole Pattern Tolerance accordion sets whether the bolt passes through both parts and takes a nut, or threads into a tapped hole in one of them. That choice changes the position tolerance on the second card, not the hole size.

How to Calculate a Clearance Hole

Clearance hole sizes are not worked out from a formula. They are looked up in a standard for the nominal bolt diameter and fit class, which is what the Clearance Hole Calculator does for you.

For metric bolts, the sizes come from ISO 273, which also suggests a hole tolerance for each series, H12 for fine, H13 for medium and H14 for coarse, as the ISO 273 abstract lists. An M6 normal hole is 6.6 mm, and the H13 band adds up to 0.22 mm. The hole can then run to 6.82 mm, which leaves 0.41 mm of play on each side of the bolt.

For inch bolts, ASME B18.2.8 gives the minimum hole for each fit, which is the figure the tool shows. A 1/4 inch normal hole is 0.281 inch, exactly a 9/32 drill.

The common mistake is reaching for the nearest fraction drill on small screws. A #10 normal hole is 0.221 inch, which a #2 number drill matches exactly, while the nearest 1/64 fraction, 15/64, is 0.013 inch larger.

For inch sizes, the first card names the drill that matches the table, along with its decimal and metric size. Screws below 1/4 inch get number or letter drills, such as #5, #2 and B for a #10, while 1/4 inch and up land on fractions like 17/64 and 9/32.

Metric and Inch Clearance Hole Chart

This metric and bolt clearance hole chart covers the most used sizes from the Clearance Hole Calculator's tables, which run from M1.6 to M36 and from #0 to 1-1/2 inch. The full list for the size you pick sits in the chart accordion under the results.

The metric steps are not even. M6 gets 0.6 mm of clearance at normal fit, but M8 jumps to 1.0 mm, so a habit of drilling 0.6 mm over leaves an M8 pattern tighter than the standard intends.

Hole Position Tolerance for Floating and Fixed Fasteners

The clearance is also the room a hole has to be out of place. ASME Y14.5 Appendix B gives the floating fastener formula, used when a bolt passes through clearance holes in both parts and takes a nut.

$$T=H-F$$

Here T is the position tolerance diameter, H is the smallest hole and F is the largest fastener. An M6 normal pattern with 6.6 mm holes can hold Ø0.6 mm position tolerance, which is what the second card of the Clearance Hole Calculator shows.

When one part is tapped, the bolt is fixed in place, and the clearance is split between the two parts. The GD&T text from Goodheart-Willcox notes that this fixed fastener formula assumes a projected tolerance zone on the threaded hole or a very thin part.

$$T=\frac{H-F}{2}$$

The same M6 normal joint then allows only Ø0.3 mm on each part, and close fit halves the room again to Ø0.2 mm. The tool uses the nominal bolt diameter for F, which is slightly conservative because real bolts run a little under nominal.

Engineers on Eng-Tips quote the same Appendix B rule, and it applies to each part on its own when hole sizes differ. To check a drilled part against its callout, the True Position Calculator turns measured X and Y offsets into a position value.

Tap Drill When the Mating Part Is Threaded

If the bolt threads into the part instead of passing through, the third card of the Clearance Hole Calculator gives the tap drill. For metric threads, the tool uses the DIN 13 convention that the fastener maker Ekinsun also lists, the nominal diameter minus the pitch.

$$D_{tap}=D-P$$

That gives 5.0 mm for M6 × 1, but 6.75 mm for M8 × 1.25 and 10.25 mm for M12 × 1.75, which are not stocked drill sizes. The tool shows both figures and rounds to the 6.8 mm and 10.2 mm drills shops use, and it does the same for the M10 × 1.25 and M12 × 1.25 fine threads.

For inch threads, the tool drills for about 75% thread, the diameter minus 0.975 divided by the threads per inch. A 1/4-20 thread works out to 0.201 inch, the size of a #7 drill, and the Thread Calculator covers the full thread dimensions.

The fourth card adds the hex nut size across flats and the plain washer diameter. An M6 nut takes a 10 mm wrench, and a spot face or counterbore should be wider than the washer so it sits flat.

Clearance Hole Questions

Which fit class should I use?

Use normal fit unless there is a reason not to. Close fit suits parts that need accurate location without dowels. An M6 close hole leaves only Ø0.4 mm of position tolerance for a floating joint, so the pattern needs a fixture or CNC drilling.

Loose fit suits field assembly, coated bolts and long patterns with tolerance stack-up. An M6 loose hole of 7.0 mm allows Ø1.0 mm, but the head loses bearing area, so add a washer.

Which standard sets clearance hole sizes?

ISO 273 covers metric bolts from 1 mm to 150 mm in fine, medium and coarse series. ASME B18.2.8 covers inch fasteners from #0 to 1-1/2 inch and metric sizes from M1.6 to M100, using close, normal and loose fits.

In the Clearance Hole Calculator, the metric choice reads ISO 273 and the inch choice reads ASME B18.2.8. Metric fit names line up as fine for close, medium for normal and coarse for loose.

Is the clearance hole different for metal and wood?

Both standards size the hole from the bolt alone, so the same chart applies to a steel plate, an aluminum bracket or a wood member. What changes is how accurately you can drill the pattern.

Hand-drilled holes in wood or field-drilled steel wander more than holes from a drill press or CNC, so they suit loose fit. Machined parts can hold the smaller position tolerance that close fit needs.

How do you calculate a 3 hole PCD?

On a pitch circle, the straight distance between neighboring holes is the circle diameter times the sine of 180° divided by the number of holes. For three holes that is 0.866 times the PCD, so a 100 mm pitch circle puts the holes 86.6 mm apart.

To work back to the pitch circle from a measured hole spacing, divide by 0.866. The Bolt Circle Calculator also gives the X and Y position of every hole for any count.