A clearance hole is a hole a fastener passes through without gripping. A tap drill hole is the opposite: it is deliberately undersized so that a tap can cut a thread into the wall that is left. Almost every bolted joint needs both, and mixing them up ruins the part. This calculator handles both sides of that pairing, plus the geometry that decides whether two parts will actually line up.
Arb Digital publishes this as a shop and workshop reference. It computes published formulas from figures you supply. It deliberately does not reproduce the clearance hole tables that live in fastener standards, because the correct row depends on which standard your drawing calls out, and a table copied into a web page is a table nobody can trace back to its source.
What This Clearance Hole Calculator Does
It does three things. First, it takes an allowance for each of the three conventional fit grades and adds it to the nominal fastener diameter, giving you three finished hole diameters side by side. Second, it computes the tap drill diameter for a threaded hole from the nominal diameter, the thread pitch and the percentage of thread you are aiming for. Third, it reports the geometric consequences of the hole you chose: the diametral clearance, the radial float the fastener has inside the hole, and whether the position tolerance on a mating pair of holes can be swallowed by that float.
The allowances are inputs and they stay inputs. Clearance holes for metric fasteners are tabulated in ISO 273, Fasteners — Clearance holes for bolts and screws, which defines fine, medium and coarse series. Inch fasteners are covered by ASME B18.2.8, Clearance Holes for Bolts, Screws, and Studs. Both are maintained documents with revisions, and both are the property of the bodies that publish them. You can find the current status of the inch standard through the ASME codes and standards catalogue. Read the row your drawing points at and type the number in.
How to Use It
- Pick the thread system. Metric threads are specified by pitch in millimetres, inch threads by threads per inch. The tool converts internally so both use the same underlying formula.
- Enter nominal diameter and pitch. For an M12 × 1.75, that is 12 and 1.75. For a 3/8-16, that is 0.375 and 16.
- Set the thread engagement you want. The default is a common general-purpose figure, but read the section below on why chasing 100 per cent is a mistake.
- Type the three clearance allowances from your standard. Or switch to single-hole mode and enter one finished diameter you already have, to see what fit it actually gives you.
- Check the float against your position tolerance. The tool tells you whether two holes at opposite extremes of tolerance can still take the fastener.
The Formula and How It Is Calculated
The clearance side is simple arithmetic: hole diameter = nominal diameter + allowance. Diametral clearance is the allowance itself, and the radial float — how far the fastener can move off centre — is half of it.
The tap drill side is the interesting one, and it is a genuine formula rather than a lookup. The theoretical thread height on a 60-degree unified or metric thread means that a hole cut to the nominal minor diameter gives full thread depth. Backing off from that by a percentage of thread gives:
Metric: tap drill = D − (E / 76.98) × P, where D is nominal diameter in millimetres, E is percentage of thread and P is pitch in millimetres.
Imperial: tap drill = D − (E × 1.299) / (100 × TPI), where D is nominal diameter in inches and TPI is threads per inch.
The two constants are the same physical quantity expressed differently. The 1.299 is the theoretical single thread height factor for a 60-degree thread form, and 76.98 is its reciprocal scaled for percentage and millimetres. Both fall straight out of the thread geometry rather than being fitted to data.
Worked example against the loaded values. An M10 × 1.5 at 75 per cent engagement gives 10 − (75 / 76.98) × 1.5 = 10 − 1.461 = 8.539 mm, which is why the standard tap drill for that thread is an 8.5 mm drill. Run it in reverse and an 8.5 mm hole in that thread gives 76.98 × (10 − 8.5) / 1.5 = 77.0 per cent of thread. On the inch side, a 1/4-20 at 75 per cent gives 0.25 − (75 × 1.299) / 2000 = 0.2013 in, which is a number 7 drill at 0.201 in. The formula reproduces the classic drill selections exactly, which is the point of using it rather than memorising them.
Why 100 Per Cent Thread Is the Wrong Target
The instinct is that more thread means more strength, so you should drill as small a hole as the tap will survive. The instinct is wrong, and it is wrong by a wide margin.
Thread strength does not scale with percentage of thread anywhere near linearly. Going from 60 per cent to 100 per cent of thread adds only a small fraction to the stripping strength of the engaged length, because the shear plane through the threads is not much larger. Meanwhile the torque required to drive the tap roughly doubles over that same range, because the tap has to displace and cut far more material at the deepest, most constrained part of the cut.
The practical consequences show up as broken taps, torn threads in soft alloys, and oversized threads caused by a tap wandering under load. In a tough material or a deep blind hole, a lower percentage of thread is not a compromise, it is the correct engineering choice, a point made at length in the NASA Fastener Design Manual. Where a joint genuinely needs more strength, the productive lever is engaged length, not percentage of thread: a thread engaged over one and a half diameters in aluminium carries far more than a shallow hole at maximum percentage. The bolt torque calculator covers what happens on the tightening side of the same joint.
Fit Grades, and What They Are Actually For
The three grades are not a quality ladder where close is best. They solve different problems.
A close fit minimises the movement between parts before the fastener is tightened. That matters where the fastener locates as well as clamps, where a hole pattern is short and made in one setup, or where the joint sees shear and you want the shank bearing early rather than after a slip. The price is that everything must be made accurately, because there is very little room to absorb error.
A normal fit is the general-purpose choice for ordinary work, and it exists because ordinary parts drift. It gives enough float to absorb realistic hole position error over a modest pattern.
A loose fit is for structural steelwork, fabrications, long hole patterns, parts made in different shops, and anything that will be assembled outdoors. It also matters for thermal movement: a long steel rail bolted to a different material will change length relative to it, and a loose hole or a slot is what stops that from tearing the joint apart.
The mistake worth naming is specifying close fits everywhere as a default. It converts an assembly problem into a manufacturing problem, and it usually gets solved on site with a drill anyway.
Position Tolerance Is What Really Sizes the Hole
Here is the calculation people skip. Two parts are bolted together. Each has a hole that may sit up to a stated distance from true position. In the worst case the two holes drift in opposite directions, so the total misalignment is the sum of both tolerances, and the fastener has to fit through both.
For the fastener to pass, the diametral clearance must be at least the sum of the two position tolerances. In other words, a clearance of 1 mm on both parts tolerates only 0.5 mm of total drift before you are wedging the bolt in. The tool applies your position tolerance to both parts and says whether the normal fit hole survives it.
This is why hole patterns fail more often than single holes. Tolerance stacks along a row, so the last hole in a line of ten can be far out of position relative to the first, even when every hole individually passed inspection. It is also why slots exist. If one hole in a pattern is slotted, the pattern locates on the round hole and the slot absorbs the accumulated error, which is a far cheaper answer than tightening every tolerance on the drawing. Our bolt circle calculator gives the true positions for a circular pattern, and the angle cut calculator covers the layout angles that put a hole where the drawing says it should be.
Countersinks, Counterbores and Material Left Behind
A clearance hole is rarely the whole feature. A countersunk screw needs a conical seat, and the countersink diameter is set by the head angle and the head diameter, not by the clearance hole. Cut it too deep and the head sinks below the surface and loses bearing area; too shallow and the head stands proud and the joint never pulls flat. A socket head cap screw in a counterbore needs the bore diameter to clear the head with a working margin and the depth to leave the head either flush or safely below the surface.
Both features remove material around the hole, and that is the part that gets forgotten in thin plate. A countersink in a 3 mm plate for an M6 screw can leave almost no parent metal under the head, at which point the joint bears on a knife edge and the plate deforms. If the plate is thin, the answer is a pan head, a washer, or a thicker local boss, not a deeper countersink. The bend allowance calculator covers the neighbouring sheet-metal arithmetic, and the carbon equivalent calculator matters if that plate will also be welded.
Where Drill Size and Hole Size Part Company
A drill does not make a hole its own size. A twist drill in a hand-held machine typically cuts oversize, and how much depends on the drill's condition, the point grind, the rigidity of the setup, the material and whether a pilot was used. In a soft, gummy material the hole can come out noticeably larger than the drill. That is fine on a clearance hole, where you have margin. It is not fine on a tap drill hole, where an oversize hole directly reduces the percentage of thread you end up with.
This is the argument for reaming, or for boring on a machine with a rigid setup, wherever the hole size actually matters. It is also an argument for running the tool in reverse: measure the hole you got, type it in as the finished diameter, and read the engagement you actually achieved rather than the one you intended.
Arb Digital builds free calculators and interactive tools that earn search traffic for engineering, fabrication and construction businesses. Browse the full library, or tell us what your customers keep asking you to work out.
Browse Free Tools Talk To Arb DigitalCommon Mistakes to Avoid
- Drilling a clearance hole where a tap drill was meant — the two differ by roughly a pitch and a half on a typical thread, and the part is scrap once it is done.
- Chasing 100 per cent thread — it adds very little strength and roughly doubles tapping torque, which is how taps break in blind holes.
- Ignoring position tolerance — two mating parts each drifting to opposite limits need clearance equal to the sum of both tolerances, not one of them.
- Using a close fit as a default — it pushes cost into manufacturing to solve a problem that a normal or loose fit solves for nothing.
- Assuming the hole is the drill size — drills cut oversize, and on a tap drill hole that loss goes straight into lost thread engagement.
Related Free Tools From Arb Digital
Pair this with the bolt torque calculator for tightening, the bolt circle calculator for hole patterns on a circle, the angle cut calculator for layout angles, the bend allowance calculator for formed parts and the carbon equivalent calculator for weldability. The full free online tools hub lists every calculator we publish, and the Arb Digital blog covers how these pages get built.
Frequently Asked Questions
A clearance hole is larger than the fastener so it passes straight through without gripping. A tap drill hole is smaller than the nominal diameter, so material is left for a tap to cut a thread into. On a typical thread they differ by roughly one and a half times the pitch.
Because the correct clearance depends on which standard your drawing invokes, and those tables belong to the bodies that maintain them. Metric holes are tabulated in ISO 273 and inch holes in ASME B18.2.8. Read the allowance from the document that governs your work and enter it.
The tool does not prescribe one. What the geometry shows is that strength rises very little above roughly three quarters of full thread while tapping torque rises sharply, so shops generally work well below 100 per cent. Where more strength is needed, more engaged length is the effective lever.
Yes. Switch the selector to single-hole mode and enter the measured diameter. The tool inverts the same formula and reports the percentage of thread that hole gives for the pitch you entered.
At minimum, enough diametral clearance to absorb the position tolerance of both mating parts added together. Over a long pattern the tolerances stack, so the far end of a row drifts much further than any single hole does, which is why one slotted hole is often the cheaper fix.
No. Twist drills cut oversize by an amount that depends on the drill condition, the point grind, the rigidity of the setup and the material. That is tolerable on a clearance hole and costly on a tap drill hole, where it comes straight out of thread engagement.
Not on its own. In a properly tightened joint the load is carried by friction from clamping, not by the fastener shank. A close fit matters where the fastener also locates the parts or where slip before bearing is unacceptable, and it costs accuracy everywhere else.
Often not. A short thread in a soft alloy strips before the fastener yields, and thin plate has nowhere to put a thread at all. Threaded inserts, weld nuts, rivet nuts and through-bolting with a nut are the usual answers, and each is a design decision rather than a drilling one.
This tool computes published thread and fit geometry from figures you supply, for reference and preliminary work only. It publishes no clearance hole table and prescribes no fastener. Fastener selection, hole specification and any joint that carries load must follow the standards invoked by your drawing and be verified by a qualified engineer.
