Drill Bit Size Chart: Number, Letter, Fractional and Metric

How to use the tools on this page

The first tab is the chart, and it does one thing no printed chart can. Type any number into the search box, a decimal like 0.201, a fraction like 1/4, a gauge like number 7, a letter, or a metric size, and it finds the nearest drill above and below in every system at once. That is the question most people actually arrive with: I need this diameter, what do I own that is closest.

The second tab works out tap drills, and it computes them rather than looking them up. Pick a thread or type a major diameter and a pitch, choose how much thread engagement you want, and it derives the exact hole diameter from the geometry of the thread form, finds the nearest real drill, and tells you what percentage of thread that drill actually produces. It also shows the next size either side, because the target almost never lands on a size that exists.

That computation is worth trusting for a specific reason. Run it across the standard threads and thirty four of thirty six computed picks come out identical to the values printed on every shop chart. The two that differ are metric sizes where the target falls almost exactly between two drills a tenth of a millimetre apart, and published charts disagree with each other on those same two rows.

The third tab is clearance holes, to the fastener standard rather than to a workshop poster, and the difference between those two is larger than you might expect.

The fourth tab is speeds and feeds, with the spindle speed plotted against drill diameter so you can see the curve rather than reading a cell.

The last tab is about why there are four systems at all, and it contains the chart that explains most of the frustration people have with drill sets: a bar for every step in the number series, showing that the series is not designed and that its two coarsest gaps sit exactly where the most commonly tapped small threads need a drill.

Four systems, and only one of them was designed

A full drill index holds sizes from four separate naming schemes that overlap, interleave and occasionally duplicate one another. None of them was planned to work with the others.

Fractional

Sixty fourths of an inch, running from 1/64 up through 1 inch and beyond in coarser steps. It is the only system with an obvious logic, and it is also the coarsest of the four. One sixty fourth is 0.397 millimetres, which is a wide step when you are trying to land on a computed tap drill target.

Number gauges, 1 to 80

Descended from the nineteenth century Stubs steel wire gauge, and the important thing about them is that there is no formula.

This is worth dwelling on, because the neighbouring system that everyone assumes is similar is nothing of the sort. American Wire Gauge is a clean geometric series: one equation gives you every diameter, and the ratio between adjacent sizes is constant. Drill number gauges are not that. The steps range from one thousandth of an inch to eight and a half thousandths and they do not vary smoothly. Plot them and you get a jagged mess rather than a curve.

The consequences are practical. Number 34 and number 35 are one thousandth apart, which is inside the tolerance of the drills themselves. So are number 45 and 46. Number 5 and number 6 are fifteen ten thousandths apart. Those near duplicates exist because two historical gauge tables were reconciled, not because anyone needed both.

More importantly, the coarsest part of the whole series sits between number 29 and number 31, where the steps are 0.0075 and 0.0085 inches. That is exactly where the tap drills for 6 32 and 8 32 fall, which is a large part of why those two threads give some of the worst engagement fits on the chart. There is no better drill to offer. A better drill does not exist.

A worked comparison against the wire gauge

The contrast with American Wire Gauge is worth making explicit, because the two systems look alike and behave nothing alike.

Wire gauge is generated by one equation, so the ratio between adjacent sizes is constant at 1.12293 and every size is 26 percent larger in area than the next one up. Knowing that one ratio reconstructs the entire table.

Drill numbers have no ratio. Between number 1 and number 2 the diameter drops 3.1 percent. Between number 30 and number 31 it drops 6.6 percent. Between number 34 and 35 it drops 0.9 percent. There is no pattern to memorise because there is no pattern.

The practical difference is that you can reason about wire gauge in your head and you cannot reason about drill numbers at all. Every drill number is a lookup, which is why the search box on this page exists.

Letters, A to Z

The same Stubs lineage, also irregular, covering the range immediately above where the number series stops. Steps run from four to fourteen thousandths and grow roughly with diameter, so the letter series is less erratic than the numbers without being systematic either.

Two facts about it are worth carrying around. The letter and number series never overlap: number 1 is 0.2280 inches and A is 0.2340, so the letters begin above where the numbers end, with a six thousandth gap between them bridged only by the fractional fifteen sixty fourths. Neither series is redundant, which is why a full index needs both.

And letter E is 0.2500 inches, exactly a quarter inch. It is the only exact duplicate anywhere in the whole system. Letter K at 0.2810 and nine thirty seconds at 0.28125 are a quarter of a thousandth apart, which is close enough to be a duplicate in practice without being one on paper.

Metric

Metric drills follow ISO 235, and even that standard does not use a single increment. The series steps by 0.02 and 0.03 millimetres below one millimetre, by 0.05 up to three millimetres, by 0.10 up to fourteen, and by 0.25 above that. The standard states outright that the range is subdivided into bands taken from the preferred number series rather than using one uniform step.

Commercially it is messier still. Most jobber sets stop at 13 millimetres because that is a common chuck capacity, and many catalogue ranges above 13 step by half a millimetre rather than a quarter.

Where the four systems leave holes

Put all four on one scale and the coverage is very uneven.

Below six millimetres you have number drills packed tightly, and the combined set is dense enough that you can usually get within a couple of hundredths of a millimetre of anything. Between six and about ten and a half millimetres the letters take over, and coverage is still reasonable. Above ten and a half millimetres both the number and letter series have run out, and the inch side has nothing but sixty fourths.

That is where the worst mismatches live. A sixty fourth is 0.397 millimetres wide, so a metric size in that band can sit almost 0.2 millimetres from the nearest inch drill, which is the largest isolation anywhere in the combined set. Twelve and a half millimetres, twelve point nine, nineteen point two five: all of them are essentially 0.2 millimetres from anything you own in inches.

The reverse problem is much milder, because above three millimetres the metric steps are finer than sixty fourths. The worst inch sizes sit about 0.12 millimetres from the nearest metric drill.

There are also about two dozen pairs that agree to within a hundredth of a millimetre, which is inside the tolerance of the drill itself. Number 47 and 2.0 millimetres. Number 25 and 3.8. Number 7 and 5.1. Letter Z and 10.5. Half an inch and 12.7. Swapping one for the other in those pairs changes nothing you could measure in the finished hole, and knowing a few of them saves a lot of drawer rummaging.

Tap drills are geometry, not a lookup

The tap drill chart taped inside every toolbox lid is not a list of arbitrary conventions. Every number on it comes from one equation, and the equation comes from the shape of a thread.

Where the constant comes from

Unified inch threads and ISO metric threads share a flank angle of 60 degrees. If you extended the flanks until they met, you would get a sharp vee triangle, and the height of that triangle, measured radially, is the pitch multiplied by the square root of three over two. That is 0.86603 times the pitch, and it is usually written as H.

Real threads are not sharp. The classic American National form that the tap drill convention was built on truncates that triangle by one eighth of H at the crest and one eighth at the root, leaving three quarters of it. So the thread height is 0.75 times 0.86603, which is 0.64952 times the pitch.

A hole is a diameter, not a radius, so you need twice that. Two times 0.64952 is 1.29904.

That is the constant. Take the major diameter of the thread, subtract the fraction of full thread you want multiplied by 1.29904 times the pitch, and you have your hole. Shop charts usually print it as 0.013 times the percentage divided by the threads per inch, which is the same thing rounded, or as a division by 76.98, which is 100 divided by 1.29904.

Nothing about it is empirical. It is the geometry of a 60 degree triangle, truncated by an eighth at each end, doubled.

A worked example

Take a quarter inch twenty threads per inch, the most common thread in imperial fastening.

The major diameter is 0.2500 inches. The pitch is one twentieth of an inch. For 75 percent engagement, subtract 0.75 times 1.29904 divided by 20, which is 0.0487. That gives 0.2013 inches.

There is no 0.2013 drill. The nearest is number 7 at 0.2010, which is what every chart in the world prints for a quarter twenty, and which actually delivers 75.4 percent rather than the 75.0 you asked for.

Do the same for 3/8 sixteen. Major diameter 0.3750, pitch one sixteenth. Subtract 0.75 times 1.29904 divided by 16, which is 0.0609. That gives 0.3141. The nearest drill is 5/16 at 0.3125, which every chart prints, and which delivers 77.0 percent.

The chart is not a chart. It is this equation, evaluated once and printed.

The metric shortcut, and why it works

Metric practice has a rule of thumb that seems too simple to be right: subtract the pitch from the major diameter. M6 with a 1.0 millimetre pitch gets a 5.0 millimetre drill. M8 with a 1.25 pitch gets 6.75, rounded to 6.8 in practice. M10 with a 1.5 pitch gets 8.5.

That rule is the same equation in disguise. Subtracting exactly one pitch corresponds to 100 divided by 1.29904, which is 76.98 percent engagement. It is the 77 percent rule wearing a hat, and that is why it never disagrees with the computed value by more than one rounding step.

It also explains why the metric tap drill chart looks so much tidier than the imperial one. The metric drill series steps by a tenth of a millimetre through the relevant range, and the targets land close to those steps. The imperial series does not, which is why imperial charts have all the argument in them.

Reading the chart

Each column answers a different question and the useful one depends on what you are doing.

Inches and millimetres are the same number twice, and both are there because the question arrives in both units. A drawing in millimetres and a drill index in inches is an ordinary situation, and the conversion is where mistakes get made.

Step to the next size is the column most charts leave out and it is the one that tells you whether you have a real choice. On the metric series through the useful range it is a steady tenth of a millimetre. On the number series it swings between one and eight and a half thousandths of an inch. If the step beside your size is large, the next drill up or down is a meaningful jump and the tool will show you what it costs in thread engagement.

Closest in the other systems is what turns four separate charts into one. It gives the nearest size in each of the other three, with the gap in millimetres, so you can see at a glance whether the substitution you were about to make is inside the tolerance of the drill or a fifth of a millimetre away.

That distinction matters more than it sounds. A hundredth of a millimetre is nothing. Two tenths of a millimetre on a tap drill is several percentage points of thread engagement, and on a reamed hole it is the whole tolerance.

The search box

Typing a decimal is the fastest way in. Enter 0.201 and the tool returns the nearest drill above, the nearest below, the nearest in inches and the nearest in metric, along with how far each one is from what you asked for.

That is the shape of the real question. Very few people need to know what a number 7 drill measures. A great many need to know what to use when the drawing says 5.1 millimetres and the index in front of them is imperial.

What is actually in a drill index

Sets are sold by piece count, and the count tells you which systems are included rather than how useful the set is.

A 29 piece set is fractional only, running 1/16 to 1/2 in sixty fourths. It covers the common sizes and nothing between them, which means it cannot hit most tap drill targets.

A 60 piece set is the number series, 1 through 60. A 115 piece set is the one most people mean by a full index: 1 through 60 in numbers, A through Z in letters, and 1/16 through 1/2 in fractional sixty fourths. That combination is what makes it possible to get close to any target between about a millimetre and half an inch.

Below number 60 the drills get very fine, down to 0.0135 inches at number 80, and they are sold separately because they break if you look at them wrong. Above half an inch you are into reduced shank drills, because a half inch chuck will not hold a five eighths shank.

The reason a 115 piece set exists rather than a smaller one is the point of this whole page. The three inch systems do not overlap, and each covers a range the others do not. A fractional set alone leaves you with 0.397 millimetre steps. Adding numbers and letters closes most of those gaps, and that is the entire justification for owning three incompatible naming schemes at once.

One hundred percent thread does not exist

This is the part that surprises people who have used tap drill charts for years.

The classic thread form, the one the tap drill constant is built on, truncates the sharp triangle by one eighth at each end and keeps three quarters of it. But the modern Unified and ISO internal thread is not truncated symmetrically. Its root, on the major diameter side, is cut back by a quarter of H rather than an eighth. Crest by one eighth, root by one quarter, leaving five eighths of the triangle rather than three quarters.

Five eighths divided by three quarters is five sixths. So on the percentage scale that every chart quotes, the geometric ceiling is exactly 83 and one third percent.

There is no such thing as a 100 percent thread. The number on the scale simply cannot be reached, because the scale is calibrated against a thread form that internal threads have not used for a long time.

And the ceiling is not just theoretical

Compute the basic minor diameter of a Unified thread using the modern five eighths form and compare it against the published minimum minor diameter for a Class 2B internal thread, which is the standard fit for almost everything.

For a quarter twenty the computation gives 0.19587 and the published minimum is 0.196. For a half thirteen, 0.41673 against 0.417. For a one inch eight, 0.86468 against 0.865. Six sizes checked, every one agreeing to within four ten thousandths of an inch.

In other words the geometric ceiling and the tightest legal hole are the same thing. Run those published minimums back through the percentage formula and they come out between 83.1 and 83.8 percent, which is the ceiling to within rounding.

So a hole drilled for 100 percent thread would be smaller than the minimum in specification minor diameter. It is not merely difficult to tap. It is out of tolerance, and a thread gauge would reject it.

Two scales are in circulation, and they differ by twenty percent

Here is a trap that catches people comparing charts.

Some manufacturers and calculators measure percent of thread against the modern basic height, the five eighths figure, rather than the classic three quarters. Their constant is 1.08253 instead of 1.29904.

The same physical hole reads about 1.2 times higher on that scale. A 75 percent thread on the classic scale is around 90 percent on the modern one. Neither is wrong. They are answering different questions, and neither usually says which.

The tool on this page uses the classic scale, because that is what shop charts, tap manufacturers and Machinery's Handbook have historically used, and because it is the scale on which the familiar 75 percent target means what people think it means. If a figure here disagrees with a supplier's calculator by roughly a fifth, that is almost certainly why.

Why 75 percent became the number

The usual explanation is that 75 percent is a good compromise between strength and tapping difficulty. That is true as far as it goes, but it is not where the number came from.

Compute the 75 percent hole for any Unified thread and compare it against the midpoint of the Class 2B minor diameter tolerance band.

For a quarter twenty the formula gives 0.2013 and the band runs 0.196 to 0.207, whose midpoint is 0.2015. For 5/16 eighteen, 0.2584 against a midpoint of 0.2585. For 3/8 sixteen, 0.3141 against 0.3140. For a half thirteen, 0.4251 against 0.4255. Across the whole range from a number 6 up to one inch, the largest disagreement is fourteen ten thousandths of an inch, and most are under five.

Seventy five percent is the centre of the tolerance band. That is what it was chosen to hit.

Which makes complete sense once you see it. Drilling to the middle of the allowed range leaves symmetric room for drill runout, for the hole cutting oversize as it always does, for tool wear, and for tap wear, before the thread leaves specification in either direction. It is a manufacturing tolerance decision dressed up as a strength decision.

The strength argument, with numbers

The strength story is real but it points somewhere else entirely.

Published figures from tap manufacturers put the tradeoff bluntly. Increasing thread depth from 60 to 72 percent in mild steel roughly doubles the required tapping torque while increasing thread strength by about five percent. Another manufacturer gives the same shape: a 100 percent thread is around five percent stronger than a 75 percent thread and demands roughly three times the tapping power.

Machinery's Handbook has long stated that beyond about 60 percent engagement there is no significant increase in strength.

So torque climbs steeply and non linearly with engagement, while shear strength flattens out above roughly 60 percent. Paying double the torque for five percent more strength is a bad trade in almost every situation, and it is a spectacularly bad one in a blind hole in stainless where a snapped tap means scrapping the part.

Some tool manufacturers now recommend 60 to 70 percent rather than 75, on exactly that reasoning. That is a defensible position and the tool here will happily compute it.

The variable that actually controls strength

If you want a stronger tapped joint, thread percentage is the wrong lever. Engagement length is the right one.

Published guidance for a thread tapped at 75 percent gives the length of engagement needed to develop the full shear strength of the fastener: about half the fastener diameter in steel, a full diameter in cast iron, and a quarter more than that in brass.

Those numbers are the ones worth designing around. Doubling the depth of a tapped hole roughly doubles the thread area carrying the load, and it costs nothing extra in tapping torque per unit of depth. Raising the thread percentage from 65 to 80 buys you a few percent of strength and doubles the torque on every millimetre of that hole.

The general rule that falls out of it: if a tapped joint is failing by stripping the internal thread, drill and tap deeper. Do not drill smaller.

The percentage you should actually aim for

Given all of the above, the question becomes practical: what number do you type into the box.

Seventy five percent is the right default for through holes in ordinary materials with a cutting tap. It is what every chart assumes, it puts you in the middle of the tolerance band, and it is what the fastener was designed around.

Sixty five to seventy percent is the better choice in three situations. In hard or tough material where tapping torque is the binding constraint. In blind holes where a snapped tap means scrapping the part. And in anything you are tapping by hand, where you are the torque limit.

The strength cost of dropping from 75 to 65 is small, on the order of a couple of percent of thread shear strength. The torque saving is large. Several tool manufacturers now recommend 60 to 70 as their default for exactly this reason.

Above eighty percent is a mistake in almost every case. You are within a few percentage points of the geometric ceiling, the hole is near the tight end of the tolerance band with no room for drill oversize or tap wear, the torque is high, and you have bought perhaps two percent of strength for it.

Below sixty percent starts to cost real strength, and it is also where a fastener can strip under a torque that should have been fine. If the drill series has forced you below 60, and it does happen on a few of the awkward sizes, consider whether a helical insert or a different thread would serve better.

The sizes where the chart fights you

A handful of common threads land badly, and it is worth knowing which before you blame yourself.

The 6 32 and 8 32 threads sit in the coarsest part of the number drill series, between number 29 and number 31, where the steps are three quarters and eight and a half thousandths. There is simply no drill close to the target, so those two threads produce engagement fits well away from 75 in one direction or the other.

Several fine threads in the middle sizes land where the nearest sixty fourth is well above target, giving engagement in the mid sixties. On those, drilling a couple of thousandths under the fraction is a legitimate move if you need the strength, though it means you are no longer using a standard drill.

The very small threads have the opposite problem. On a 0 80 the available drills bracket the target so widely that the conventional choice sits above 80 percent, because the next size down would exceed the ceiling and the one after that would collapse to under 50.

None of that is a flaw in the calculation. It is what happens when a continuous target meets a discrete and irregular set of tools.

Clearance holes

A clearance hole is the through hole the fastener passes without engaging, and it is a different problem from a tap drill in every respect.

The fastener standard defines three classes. A close fit for accurate location, a normal fit for general assembly, and a loose fit where parts need room to move during alignment. Each class gives a minimum and a maximum hole diameter, not a single number.

The counterintuitive part is that clearance depends only on the nominal fastener diameter. The thread pitch is irrelevant. A quarter twenty and a quarter twenty eight take exactly the same clearance hole, because the bolt shank is the same size and the threads never touch the hole. People expect fine threads to want something different and they do not.

Workshop charts disagree with the standard

This is worth knowing before an inspector points it out.

A great many circulated clearance drill charts give noticeably tighter holes than the fastener standard does. A number 10 close fit is 0.206 inches in the standard and 0.196 on most workshop posters, which is a whole drill size difference. Those informal charts either predate the standard or ignore it, and they are perfectly serviceable for general work while being wrong if a drawing calls the standard out by number.

The tool here uses the standard values and names the nearest drill to each. If your drawing says otherwise, the drawing wins.

The step at number 5

One feature of the table looks like a data entry error and is not.

Close fit clearance runs seven to eight thousandths over nominal for sizes 0 through 4, then jumps to sixteen thousandths from number 5 upward and stays there through a quarter inch. The jump is real and it is in the standard.

Speeds, feeds and why the numbers disagree

The formula

Spindle speed in revolutions per minute is 3.81972 multiplied by the surface speed in feet per minute, divided by the drill diameter in inches.

The constant is not a fudge. The cutting edge travels one circumference per revolution, which is pi times the diameter in inches. Surface speed is quoted in feet per minute. So you divide by pi to convert circumference to revolutions and multiply by twelve to convert feet to inches, and twelve divided by pi is 3.81972.

The shop shortcut of four times the surface speed over the diameter is that constant rounded up. It runs 4.7 percent fast, which is inside the noise on most jobs and worth knowing about on none.

In metric the same derivation gives 318.31 times the cutting speed in metres per minute, divided by the diameter in millimetres, the 1000 replacing the 12.

Why published speeds disagree so wildly

Compare surface speed tables from different manufacturers and you will find disagreements of up to three times on the same material. That is not sloppiness. It reflects genuine variation in what the tables assume about coolant, rigidity, hole depth, drill coating and how long a tool life the author considers acceptable.

The pattern that survives across all of them is the ordering. Aluminium runs fastest, at two to three hundred surface feet per minute in high speed steel. Mild steel is roughly a third of that. Stainless in the 300 series is a third again, at twenty to forty, because it work hardens and traps heat. Hardened steel, titanium and the nickel alloys are slower still.

Carbide roughly doubles the figure in steels, but the multiplier is not general. In aluminium the carbide advantage is much smaller because high speed steel is already running fast, and a blanket rule of two and a half times overpredicts badly there.

Feed rates disagree by about a factor of two between published tables. A rule that lands in the middle of all of them is about two percent of the drill diameter per revolution, which gives five thousandths at a quarter inch, ten at a half, and twenty at an inch.

Point angles

The angle ground on the tip changes the behaviour of the drill more than most people expect.

A 118 degree point is the standard general purpose grind. It is sharper, has a shorter chisel edge, cuts more aggressively and needs less push. It also walks on a flat unpunched surface, and its thinner tip dulls quickly in hard material.

A 135 degree point is blunter, with a wider chisel edge, so it needs more axial thrust to start cutting. In exchange the corner carries more material and survives far longer in hard or work hardening material, and it grips better on curved surfaces. It is the default for stainless, titanium, hardened steel and the nickel alloys.

A split point adds two extra cutting edges ground into the chisel edge, thinning the web. The chisel edge stops extruding material and starts cutting it. The result is self centring, needs no pilot hole and cuts thrust sharply. The tradeoff is that it cannot be resharpened freehand.

Two recommendations in the tables look like typos and are not. Ninety degrees for soft grey cast iron and 111 for brass. Both are aimed at controlling the grabbing, self feeding behaviour those materials show with a standard grind, where the drill tries to screw itself into the work as it breaks through.

Getting the hole where you wanted it

A drill produces a hole larger than itself, out of round and not quite where you aimed. All three are normal and all three are manageable.

Oversize is the least avoidable. A two flute twist drill is self guiding only after the full diameter is engaged, and any imbalance between the two lips steers it. A hole a thousandth or two over nominal is ordinary, and more than that usually means the lips are ground unequally.

That matters directly for tapping. If your tap drill cuts two thousandths oversize, the thread percentage falls by roughly the same amount it would if you had deliberately chosen the next drill up. On a fine thread, two thousandths can be five or six percentage points of engagement. It is worth measuring a test hole before committing on a part you cannot replace.

Walking is the positional problem, and the fix is to remove the need for the drill to find its own centre. A centre punch, a spot drill, or a split point all do the same job by different means. A spot drill is stiff and short and cuts a shallow conical seat that the twist drill then follows, and it is the most reliable of the three on a machine.

Peck drilling matters once the hole gets deeper than about three diameters. Chips have to travel back up the flutes, and past that depth they stop clearing reliably, pack, and either break the drill or weld themselves to it. Retracting periodically clears them and lets coolant reach the tip.

Through holes need care at breakout. The moment the point emerges, the resistance drops and the feed suddenly has nothing to push against, which is when a drill grabs, snatches the work, or splinters the far side. Easing off just before breakout is the fix.

What the drill is made of

The size chart says nothing about what will actually survive the material you are cutting, and that is a separate decision with real consequences.

Carbon steel is the cheapest and the least useful. It loses hardness at low temperature, so it is fine in wood and soft plastics and hopeless in metal at any sensible speed.

High speed steel is the baseline for metalworking. It holds its edge to around 600 degrees, which is enough for most drilling, and it is tough enough to survive a bit of chatter and a slightly wandering machine. Almost every general purpose drill is high speed steel.

Cobalt, usually sold as M35 or M42 depending on how much cobalt is in the alloy, is high speed steel with five or eight percent cobalt added. It runs hotter before softening, which matters specifically in stainless, titanium and anything that work hardens. It is also more brittle, so it chips rather than blunts if the setup flexes. Cobalt in a hand drill is often a waste of money for that reason.

Carbide is a different class again. It runs at roughly double the surface speed of high speed steel in steels, holds an edge far longer, and is unforgiving. It has almost no toughness, so any deflection, any runout, any interrupted cut without a rigid setup, and it shatters. Carbide belongs in a machine, not in a hand drill.

Coatings

Coatings change surface behaviour, not the substrate. A coated high speed steel drill is still high speed steel underneath.

Black oxide is barely a coating. It reduces friction slightly and resists corrosion, and it costs almost nothing. It is a marginal improvement over bare high speed steel.

Titanium nitride, the gold coloured one, is genuinely harder and slicker than the steel underneath and extends life meaningfully in steel and iron. It is thin. Once it wears through at the cutting edge, and it wears through first exactly where the work happens, you are back to bare high speed steel. It also cannot be resharpened without removing it.

Titanium aluminium nitride and its relatives are the ones that matter for hard and hot work. They form a thin aluminium oxide layer at temperature that insulates the tool, which is the opposite of what most coatings do and is exactly what you want when you cannot get coolant to the tip.

The trap with coated drills is the resharpening one. A coating lives on the surface. Grind the point and the coating is gone from the only part that was doing anything.

Drilling specific materials

Each common material fails in its own particular way, and knowing the failure mode is more useful than knowing the surface speed.

Mild steel

The easy case. Standard 118 degree point, moderate speed, any cutting fluid, and it will produce long continuous chips that need clearing on deep holes. If it is squealing, the speed is too high or the feed too light and the drill is rubbing instead of cutting.

Stainless, 300 series

The one that catches everyone. Austenitic stainless work hardens under a rubbing tool, which means a drill that is going too fast, feeding too lightly, or dwelling at the bottom of a hole will glaze the surface into something considerably harder than the material you started with. After that it will not cut at all.

The rules are the opposite of instinct. Slow down, twenty to forty surface feet per minute rather than the hundred you would use in mild steel. Feed harder, not softer. Never let the drill spin without advancing. Use a 135 degree point, use cobalt if you have it, and keep the cut flooded.

Aluminium

Fast, and prone to two specific problems. Aluminium is soft enough that it welds to the cutting edge, building up a lump that changes the geometry and tears the hole. And a standard drill grind will grab and self feed as it breaks through, snatching thin material out of your hands.

Cutting fluid helps with the first, and so do polished flutes and higher helix angles. The second is handled by easing off at breakout, or by clamping properly, or by using a slower helix drill made for the job.

Cast iron

Grey cast iron produces powder rather than chips, which is why it is normally drilled dry. The graphite in it is a lubricant of sorts. The powder is abrasive and it gets into everything, including the machine ways.

It also tends to grab at breakout because of the graphite it contains, which is why some manufacturers recommend a 90 degree point for soft grey iron specifically, to stop the drill screwing itself into the work.

Brass and bronze

Brass is where a standard drill grind is actively dangerous. Brass is soft but has almost no elasticity, so a sharp positive rake edge digs in and pulls the drill through the material. On a drill press it can snatch the part. On a hand drill it can wreck the hole.

The fix is to reduce the rake, which is what the unusual 111 degree point recommendation in the tables is about. A common workshop version is to take the edge off the cutting lip with a stone, deliberately dulling it slightly.

Plastics

Governed by melt temperature far more than by surface speed. Too fast and the material melts, welds behind the drill and grabs. Acrylic in particular will crack rather than cut if the drill is dull or the feed uneven.

Slow speeds, sharp tools, clear the chips often, and back the material with a sacrificial piece to prevent breakout chipping.

Wood

A twist drill works in wood but a brad point or Forstner does it better, because the outer rim scores the fibres before the centre removes them, which is what stops tearout on the entry side. On the exit side, back the workpiece.

Speeds are diameter dependent and the tables give revolutions rather than surface speed. Converting them puts hardwood at roughly a hundred to a hundred and fifty surface feet per minute, comparable to cast iron in high speed steel, with softwood about double.

Pilot holes for screws, which is a different problem again

Machine screws go into tapped holes. Wood screws and sheet metal screws do not, and sizing their holes follows different logic.

A wood screw needs two holes of different diameters. The shank hole through the upper piece should clear the unthreaded shank entirely, so the screw can pull the two pieces together. The pilot hole in the lower piece should match the root diameter of the thread, so the threads have material to bite while the screw is not trying to split the wood.

Skip the shank hole and the screw threads grip the upper piece as well as the lower one, which means it cannot draw the joint closed. The pieces stay apart with the screw spinning happily between them. That is the single most common wood screwing mistake and the fix costs one extra drill.

The pilot diameter depends on the wood. Hardwood needs a pilot close to the root diameter, because there is no compliance to spare and the screw will split it. Softwood tolerates a pilot noticeably smaller, and in some softwoods small screws need no pilot at all. End grain is a case of its own: it holds badly no matter what you do, and a pilot sized for face grain will often split it.

Self tapping and sheet metal screws form or cut their own thread in a hole sized between the root and major diameters, and the manufacturer's own table is the only reliable source, because the thread forms vary far more than machine screw threads do.

Thread forming taps want a bigger hole

Everything above assumes a cutting tap, which removes material to make a thread. Thread forming taps, also called roll taps or cold forming taps, do not cut. They displace material, pushing it up into the thread form.

That changes the hole size substantially. Because nothing is removed, the material has to come from somewhere, and it comes from the wall of the hole moving inward. A forming tap therefore needs a noticeably larger starting hole than a cutting tap for the same thread.

The published relation subtracts the percentage multiplied by the pitch divided by 175, rather than divided by 76.98. For an M6 by 1.0 at 65 percent that gives 5.63 millimetres, against 5.0 for a cutting tap. That is a large difference and using a cutting tap drill with a forming tap will break the tap.

Forming taps also target lower engagement, typically 60 to 70 percent rather than 75, and they are usually restricted to ductile materials. Aluminium, copper, brass, low carbon steel and austenitic stainless all form well. Cast iron and anything brittle does not, because the material cracks rather than flowing.

The upside is real. A formed thread has no chips to evacuate, which makes blind holes far easier, and the grain flow follows the thread contour rather than being cut through, which produces a measurably stronger thread. Tap life is also usually much longer.

Breaking taps, and how not to

A snapped tap in a nearly finished part is one of the more expensive ways to spend an afternoon, and most of the causes are avoidable.

Drilling the hole too small is the obvious one and it is the reason for everything above. Every percentage point of extra engagement is more material for the tap to remove and more torque on a tool that is essentially a hardened, fluted, brittle screw.

Not clearing chips in a blind hole is the next. A cutting tap makes chips that have nowhere to go once the hole bottoms out, and they pack under the tap and jam it. Spiral point taps push chips forward, which works in a through hole and makes the packing worse in a blind one. Spiral flute taps pull chips back out and are the right choice for blind holes.

Tapping to the bottom is a related error. The lead threads on a plug tap cut nothing at full depth, so the last few threads of the drilled hole are not usable anyway, and driving the tap down until it stops is how you find out. Drill deeper than the thread depth you need.

Misalignment loads one side of the tap. A tap started even a couple of degrees off will cut unevenly, and the correction it experiences as it straightens itself is a bending load on a brittle tool. A tapping guide, a tailstock centre, or simply starting under power in the machine that drilled the hole all remove this.

And on the far end: hard material with a cutting tap and no lubricant, in a blind hole, at 80 percent engagement, is asking for it. That is where forming taps and lower engagement targets earn their money.

When a drilled hole is not accurate enough

A drill makes a hole that is oversize, slightly out of round, not perfectly straight and not exactly where you aimed. For most work that is fine. For a bearing fit, a dowel pin, or anything with a tolerance in the tenths of a thousandth, it is not.

Reaming is the usual next step. A reamer is not a drill: it does not create a hole, it finishes one. It takes a small, even amount off an existing hole and leaves a size and finish a drill cannot. The standard practice is to drill undersize by roughly a sixty fourth for holes up to half an inch, or a thirty second above that, then ream to size.

Reaming will not fix position. A reamer follows the hole it is given, so a hole that wandered stays wandered, just rounder. Fixing position means boring, which uses a single point tool that cuts to wherever the machine tells it rather than following the existing hole.

For a dowel pin hole the sequence is spot drill, drill undersize, then ream. Skipping the spot drill costs you position, skipping the undersize step leaves the reamer nothing to cut, and asking a reamer to remove too much makes it chatter and produces a worse hole than the drill did.

What is taught wrong about drill sizes

That the number series follows a pattern

It does not. Unlike American Wire Gauge, which is a geometric series generated by one formula, drill number gauges are an irregular historical list. Steps range from one to eight and a half thousandths of an inch and jump around unpredictably. There are near duplicate sizes a thousandth apart, and the two coarsest gaps in the whole series sit exactly where the 6 32 and 8 32 tap drills need to be.

That 100 percent thread engagement is achievable

The geometric ceiling on the scale everyone quotes is 83 and a third percent, because modern internal threads keep five eighths of the fundamental triangle rather than three quarters. A hole drilled for 100 percent would be below the minimum in specification minor diameter. It is out of tolerance, not just hard.

That 75 percent is the strength optimum

It is the midpoint of the Class 2B minor diameter tolerance band, which is a manufacturing tolerance choice. On strength grounds, published figures show no significant gain above about 60 percent, while torque roughly doubles going from 60 to 72 percent for about five percent more strength.

That a tighter tap drill makes a stronger joint

It makes a marginally stronger thread and a much harder tapping operation. If a tapped joint is stripping, the answer is depth. Half a fastener diameter of engagement in steel, a full diameter in cast iron, more in brass. Doubling the depth roughly doubles the thread area carrying load. Raising thread percentage buys single digit percentages.

That fine threads need different clearance holes

Clearance is set by nominal fastener diameter alone. A quarter twenty and a quarter twenty eight take the same clearance hole, because the shank is the same size and the threads never touch it.

That all percent of thread figures mean the same thing

Two scales are in circulation, differing by a factor of about 1.2. Measured against the classic three quarters height, a hole reads 75 percent. Measured against the modern five eighths basic height, the same hole reads about 90. Charts rarely say which they are using.

That the same gauge number means the same thing across tools

It does not even mean the same thing within drilling. A number 10 drill is 0.1935 inches. A number 10 machine screw is 0.190 inches major diameter. A number 10 wire is something else again. The numbers are unrelated scales that happen to share notation.

That a bigger point angle is always better for hard material

It usually is, but the reason matters. A 135 degree point survives longer in hard material because the corner carries more mass, not because it cuts better. It needs more thrust to penetrate, and on a hand drill or a light bench machine that can mean it simply rubs and work hardens the surface instead of cutting. Match the grind to the machine as well as the material.

Mistakes that catch people out

Using a tap drill chart without checking which thread standard it covers. UNC, UNF, metric coarse and metric fine all exist at the same nominal diameters, and picking the wrong row gives a hole that taps beautifully and produces the wrong thread.

Forgetting that the hole cuts oversize. On a fine thread two thousandths of oversize can cost five or six percentage points of engagement, which is more than the difference between two adjacent chart recommendations.

Reading a metric tap drill chart and rounding to the nearest inch drill you happen to own without recomputing. Some of those substitutions are within a hundredth of a millimetre and some are two tenths, and the tool tells you which is which.

Tapping a blind hole to the bottom. A plug tap has several lead threads that cut nothing at full depth, so the usable thread is always shorter than the drilled depth. Drill deeper than you think you need, or use a bottoming tap for the last part.

Using clearance figures from a workshop poster on a drawing that calls out the fastener standard by number. The differences are up to a full drill size.

Assuming a letter drill and a number drill of similar size are interchangeable. They are separate series that never overlap, so if a chart specifies letter F there is no number drill anywhere near it.

Running stainless at mild steel speeds. The 300 series work hardens under a rubbing tool, so a drill that is going too slow, or that dwells without cutting, glazes the surface and then will not cut at all. The failure is not gradual.

Drilling deep holes without pecking. Past about three diameters the chips stop clearing on their own, and the failure mode is a packed flute followed by a broken drill.

Where the numbers on this page come from

Most drill charts online are transcriptions. It matters because a transcription error is silent, and there is no way to catch one by looking at it.

The sizes here come from two sources, and only one of them is a list.

Fractional and metric sizes are generated rather than typed. Sixty fourths of an inch is arithmetic. The metric series is generated from the increment bands the standard specifies: 0.02 and 0.03 below one millimetre, 0.05 up to three, 0.10 up to fourteen, 0.25 above that.

Number and letter sizes cannot be generated, because as covered above they follow no formula. Those are a list, cross checked against two independent published sources.

The tap drills are the interesting case, because they were not copied at all. Every one on this page is computed from the thread geometry: the major diameter, the pitch, the 60 degree form, the three quarter truncation, and the target percentage. The tool then searches the drill list for the nearest size that actually exists.

The check that makes it trustworthy

Run that computation across the standard threads and compare the results against what conventional charts print.

Thirty four of thirty six computed picks come out identical. Number 43 for a 4 40, number 36 for a 6 32, number 29 for an 8 32, number 7 for a quarter twenty, letter F for a 5/16 eighteen, five sixteenths for a 3/8 sixteen, twenty seven sixty fourths for a half thirteen. All of them fall out of the equation without a chart being consulted.

The two that differ are M12 and M14, and both are cases where the computed target lands almost exactly between two metric drills a tenth of a millimetre apart. Published charts disagree with each other on those same two rows, some printing 10.2 for M12 and others 10.3. Both are in specification. There is no right answer, only a choice.

That is a useful kind of disagreement to be able to see, and it is invisible on a printed chart.

And a check on the ceiling

The same geometry that gives the tap drill constant also gives the maximum achievable thread percentage, and that claim can be tested against a completely separate document.

Compute the basic minor diameter from the modern five eighths thread form for six Unified sizes and compare against the published minimum minor diameter for a Class 2B internal thread. Quarter twenty: computed 0.19587, published 0.196. Half thirteen: 0.41673 against 0.417. One inch eight: 0.86468 against 0.865. The largest disagreement across all six is under four ten thousandths of an inch.

Two independent routes to the same number is the point. The thread geometry and the fastener tolerance standard agree, which is what tells you the geometry is being applied correctly rather than merely consistently.

Where this page may differ from your reference

Three caveats, because a reference that does not state its limits is not one.

The size lists come from a standard that is old and stable. The number, letter and fractional drill sizes are specified in ANSI and ASME B94.11M, whose most recent edition dates from 1993 and which has not been superseded. Metric sizes follow ISO 235, revised in 2016. Neither has moved in a way that would change any figure here, which is precisely why a drill chart is worth printing at all. But commercial stock is a different question from a standard, and the metric range above thirteen millimetres in particular is often supplied in half millimetre steps rather than the quarter millimetre steps the standard lists.

Tap drill charts genuinely disagree with each other, and now you can see why. Several sizes have a computed target that falls almost exactly between two available drills, and different publishers round different ways. Number 2 56 splits between number 50 and number 51. Number 5 40 splits between 38 and 39. Number 12 24 splits between 16 and 17. M12 splits between 10.2 and 10.3 millimetres. All of those are in specification and none is wrong, which is worth knowing before you conclude that one of two charts must be in error.

One case is worth flagging specifically. Some published charts give number 51 for a 2 56, which computes to 84.5 percent engagement. That is above the geometric ceiling of 83 and a third, which means the resulting hole would be tighter than the minimum in specification minor diameter. The tool here will not offer it.

Speeds and feeds are recommendations, not specifications. Surface speed figures from different manufacturers differ by up to three times on the same material, and feed tables by about two. Those are not errors. They reflect different assumptions about coolant, rigidity, hole depth, coating and acceptable tool life, none of which the table states. Treat everything on the speeds tab as a starting point and adjust to what the cut is telling you.

The geometry does not depend on any of that. The thread form, the tap drill constant, the 83 and a third percent ceiling and the RPM formula are all consequences of arithmetic rather than of committee decisions, and they will not change.

Common questions about drill bit sizes

What are the four drill bit size systems?

Fractional, in sixty fourths of an inch. Number gauges from 1 to 80, where a bigger number means a smaller drill. Letters A through Z, which cover the range just above where the number series ends. And metric, specified directly in millimetres under ISO 235. They interleave and overlap and only the fractional series has an obvious internal logic.

Why do bigger drill numbers mean smaller drills?

Because the number series descends from the Stubs steel wire gauge, where the number counted stages in a wire drawing process rather than measuring anything. Each stage made the wire thinner. The convention survived into drill sizing even though drills are not made that way.

Is there a formula for drill number sizes?

No. This is the difference between drill gauges and American Wire Gauge, which people often assume are similar. AWG is a clean geometric series generated by one equation. Drill number sizes are an irregular historical list, with steps ranging from one thousandth of an inch up to eight and a half thousandths, changing unpredictably along the series.

What size drill do I need for a quarter twenty tap?

A number 7 drill, 0.2010 inches. That comes out of the formula rather than a chart: major diameter 0.2500 minus 0.75 times 1.29904 divided by 20 gives 0.2013 inches, and number 7 is the nearest drill that exists. It actually produces 75.4 percent thread engagement.

How do I calculate a tap drill size?

Subtract from the major diameter the percentage of thread you want, divided by 100, multiplied by 1.29904, multiplied by the pitch. For inch threads the pitch is one over the threads per inch, so the formula becomes major diameter minus percentage times 0.0129904 divided by threads per inch. The constant comes from the 60 degree thread form, not from a table.

Where does the tap drill constant 1.29904 come from?

From geometry. A 60 degree thread is cut from a triangle whose height is the pitch times the square root of three over two, or 0.86603 times the pitch. The classic thread form truncates it by an eighth at the crest and an eighth at the root, keeping three quarters, which is 0.64952 times the pitch. A hole is a diameter, so you double it, giving 1.29904.

Why is 75 percent thread engagement the standard target?

Because it lands on the midpoint of the Class 2B minor diameter tolerance band. Compute the 75 percent hole for any Unified thread and it agrees with that midpoint to within about a thousandth of an inch across the whole size range. It is a manufacturing tolerance decision, not a strength optimum, and drilling to the middle of the band leaves symmetric room for drill runout, oversize cutting and tap wear.

Can you get 100 percent thread engagement?

No. Modern internal threads keep five eighths of the fundamental triangle rather than three quarters, so on the percentage scale that every chart uses the geometric ceiling is exactly 83 and one third percent. A hole drilled for 100 percent would be smaller than the minimum in specification minor diameter, which makes it out of tolerance rather than merely difficult to tap.

Is a deeper thread stronger?

Barely, and it costs a great deal. Published manufacturer figures show that going from 60 to 72 percent engagement roughly doubles the tapping torque for about five percent more thread strength, and Machinery's Handbook has long said there is no significant strength gain above about 60 percent. If you need a stronger tapped joint, tap deeper rather than smaller. Half a fastener diameter of engagement in steel, a full diameter in cast iron.

What is the metric rule of subtracting the pitch?

Take the major diameter and subtract the pitch. M6 with a one millimetre pitch takes a five millimetre drill, M10 with a 1.5 pitch takes 8.5. It works because subtracting exactly one pitch corresponds to 76.98 percent engagement on the standard scale, which is close enough to 75 that the two rules never disagree by more than one rounding step.

What is the difference between a tap drill and a clearance hole?

A tap drill is the hole you cut threads into, sized so the tap leaves a specified percentage of thread. A clearance hole is a through hole the fastener passes without engaging at all, sized only by the nominal fastener diameter. Thread pitch is irrelevant to a clearance hole, which surprises people who expect fine threads to need something different.

Which drill sizes are the same in inch and metric?

About two dozen pairs agree to within a hundredth of a millimetre, which is inside the tolerance of the drills themselves. Number 47 and 2.0 millimetres. Number 25 and 3.8. Number 7 and 5.1. Letter Z and 10.5. Half an inch and 12.7. In those cases substituting one for the other changes nothing measurable in the hole.

What is the difference between a 118 and a 135 degree drill point?

A 118 degree point is sharper, has a shorter chisel edge and needs less thrust, which suits general work in mild steel, aluminium, wood and plastics. A 135 degree point is blunter and needs more thrust, but the corner carries more material so it survives far longer in stainless, titanium, hardened steel and the nickel alloys. A split point, usually paired with 135 degrees, grinds cutting edges into the chisel edge so the tip cuts instead of extruding, making it self centring and cutting the thrust needed.

How do I calculate drill RPM?

Multiply the surface speed in feet per minute by 3.81972 and divide by the drill diameter in inches. The constant is twelve divided by pi: twelve converts feet to inches and pi converts circumference to revolutions. The common shortcut of four times surface speed over diameter is that constant rounded up and runs about 4.7 percent fast.

Why do drill speed charts disagree so much?

Because they assume different things about coolant, machine rigidity, hole depth, drill coating and how much tool life is acceptable. Published surface speeds for the same material can differ by up to three times between manufacturers. What survives across all of them is the ordering: aluminium fastest, mild steel about a third of that, 300 series stainless a third again, and the hardened and nickel alloys slower still.

Why does my drilled hole come out oversize?

Because a two flute twist drill only guides itself once the full diameter is engaged, and any imbalance between the two cutting lips steers it. A thousandth or two over nominal is normal. More than that usually means the lips are ground unequally. It matters for tapping, because two thousandths of oversize on a fine thread can cost five or six percentage points of engagement, which is more than the gap between two adjacent chart recommendations.

Related Calculators and Reference

• Wire Gauge Chart with AWG Sizes and Ampacity is the system drill numbers are constantly confused with, and the contrast is instructive: wire gauge is a clean geometric series generated by one equation, drill gauges are an irregular historical list.
• Length Converter handles the inch and millimetre conversions behind every substitution decision on this page.
• Decimal to Fraction Converter turns a decimal diameter into the nearest fractional drill size and tells you how far off it is.
• Torque Unit Converter covers the units the tapping torque figures on this page get quoted in.
• Modulus of Elasticity of Steel gives the stiffness values behind the material behaviour that decides cutting speeds.
• ASME B94.11M is the standard that fixes the number, letter and fractional drill sizes used here.
• ISO 235 is the metric equivalent, and the source of the increment bands the metric series follows.