Tap Drill Size Chart

How to read a tap drill chart

Every row on a tap drill chart answers one question: given this thread, what hole do I drill before I run the tap in? The answer is always a hole smaller than the bolt. The tap's job is to cut a thread into the wall of that hole, and it needs material to cut into. If the hole were bolt-sized there would be nothing left to make a thread out of.

Take 1/4-20. The bolt measures 0.250 in across the thread crests. The drill is #7, which is 0.201 in — noticeably smaller. What is left between 0.201 in and 0.250 in is the metal the tap turns into thread.

The columns after the drill size give you the same number in different forms and for different situations. Decimal inches and millimetres let you check whatever is stamped on the bit. The hard-material column is a larger drill for when the tap would otherwise have to fight. The form-tap column is larger still, for roll taps. And the percent of thread column is the one that explains all of it.

What percent of thread means

Percent of thread is how tall the thread the tap cuts is, compared with a full theoretical thread. It is not a measure of quality or of how much of the bolt is engaged along its length. It is purely the height of each thread tooth.

Every thread has a basic minor diameter: the smallest hole that still lets a full-height thread form. For 1/4-20 that is 0.1959 in. Drill exactly that and the tap would cut 100% of the thread height. Nobody does this. You drill a little larger, the tap cuts shorter teeth, and the ratio of what you got to the full height is the percent of thread.

The reason nobody drills for 100% is the trade. A 100% thread is only about 5% stronger than a 75% one, and it takes roughly three times the torque to cut. You pay triple for a twentieth more strength, and you pay it in broken taps. That is why essentially every published chart sits near 75%.

Which is also why the percent column on these charts is not a flat 75% all the way down. The published drill is a real drill you can buy, not the exact theoretical size, so the figure it lands on depends on how the drill sizes happen to fall at that pitch. 1/4-20 comes out at 75.4% and #10-32 at 76.4%. We show the figure each drill really gives rather than rounding everything to a tidy 75%.

The formulas

Four of them cover everything on this site:

• Inch percent of thread: % = 76.98 × TPI × (major − drill), in inches.
• Metric percent of thread: % = (major − drill) ÷ (0.01299 × pitch), in millimetres.
• Cut tap drill for a target percent: drill = major − 0.01299 × % × pitch.
• Form tap drill: drill = major − 0.0068 × % × pitch.

For inch threads the pitch is 1 ÷ TPI. For metric there is a shortcut worth memorising: drill = diameter − pitch gives about 77% of thread for any metric size. M6 x 1 is 6 − 1 = 5 mm, exactly the chart drill. M8 x 1.25 is 8 − 1.25 = 6.75 mm, which is not a drill anyone stocks, so charts use 6.8 mm instead.

Cut taps and form taps

A cutting tap has flutes and sharp edges. It shaves metal out of the hole, and those chips have to go somewhere: up the flutes, or ahead of the tap, or packed into the bottom of a blind hole where they will jam and snap it.

A form tap, also called a roll or fluteless tap, has no cutting edges at all. It is a hardened lobed screw that presses the thread into the hole wall. Nothing is removed, so there are no chips to manage. The displaced metal flows inward to make the crests, which means the hole has to start larger to supply it.

The difference is not subtle. 1/4-20 takes #7 (0.201 in) with a cut tap and #1 (0.228 in) with a form tap. Use the cut-tap drill with a form tap and you will break it. Form taps suit ductile material — aluminium, copper, brass, mild steel, many stainless grades — and not brittle ones like grey cast iron, where the metal fractures instead of flowing. The form tap drill chart lists every size.

Choosing a drill by material

The chart drill assumes something reasonable. When the material is not reasonable, change the hole:

• Aluminium, brass, plastic: the standard 75% drill. These cut easily, so a deeper thread costs little, and a shallower one strips sooner in soft material. Keep the tap lubricated; aluminium in particular welds itself to cutting edges.
• Mild steel and cast iron: around 70%. The standard chart drill is fine, and one size up is fine too if the tap is fighting.
• Stainless and tool steel: 60 to 65%, which is what the hard-material column on every chart gives you. Stainless work hardens when a tool rubs instead of cutting, so a tap that stalls makes its own problem worse. Less thread to cut means less torque and less heat.
• Deep holes, anything past about 1.5 diameters: drop the engagement. Torque accumulates down the hole, so what is comfortable at the top can be at the limit near the bottom.

Blind holes and through holes

A through hole is the easy case: chips can fall out of the bottom. A spiral point (gun) tap is ideal, because it deliberately pushes chips forward and out ahead of itself.

A blind hole has a bottom, and everything the tap cuts stays in there with it. Chips pack into the bottom, the tap reaches them, torque spikes and it breaks. Use a spiral flute tap, which pulls chips back up and out the top, or a form tap, which makes no chips at all. Avoid spiral point taps here, since they push chips to exactly the wrong place.

Drill the blind hole deeper than the thread you need. The first few threads on any tap are ground back into a taper (the chamfer) and cannot cut a full thread, so the bottom of a tapped hole always has incomplete threads. Add the chamfer length plus at least one more pitch, then more again for chips and for the drill point.

Five mistakes that cost taps

1. Drilling the clearance hole by mistake. If the bit is the same size as the bolt, it is the wrong bit. The tap drill is always smaller. See the clearance hole chart for the other kind.
2. Using a cut-tap drill with a form tap. Far too much metal to displace. This one usually breaks on the first hole.
3. Not backing off in a blind hole. Half a turn back for every turn forward breaks the chip and keeps the flutes clear.
4. Tapping dry. Cutting fluid is not optional, least of all in aluminium and stainless. It is the difference between a clean thread and a torn one.
5. Starting crooked. A tap that goes in off-square cuts a thread that will never take a bolt straight, and it loads one side of the tap. Start it in the drill press with the spindle unpowered, or use a tap guide.

Working out a thread you already have

You need two numbers, and the first one alone is not enough, because several pitches share each diameter.

1. Measure the major diameter over the thread crests with calipers. Expect it to read a few thousandths under nominal; a 1/4 in bolt measures about 0.245 in.
2. Find the pitch with a thread gauge. Try both inch and metric leaves. The right one sits down along the whole thread with no rocking and no light under it. Without a gauge, count crests over an inch (inch threads) or over 10 mm (metric).

That second step is what separates 1/4-20 from 1/4-28. Same diameter, different pitch, different taps, and different drills: #7 against #3.

Watch for near-misses between the systems. M6 and 1/4-20, M8 and 5/16-18, M10 and 3/8-16 are close enough in diameter to start in each other's holes and then bind solid. Every size page on this site names its nearest counterpart in the other system, with that warning attached.

The sizes people look up most

1/4-20 (#7), 5/16-18 (F), #10-32 (#21), #8-32 (#29) and M6 x 1 (5 mm) account for a large share of all tap drill searches. Each has its own page with the clearance holes, a to-scale section through the hole, a calculator pre-filled with that thread, and a card you can print and keep by the machine.

Where these numbers come from

The tap drills on this site are the published chart sizes, not values invented here. Every percent of thread was recomputed from that size's own major diameter and pitch with the formulas above, and the build fails if a stored figure and a recomputed one disagree by more than 0.2. Inch clearance holes follow ASME B18.2.8 and metric ones ISO 273. Where a size falls outside those standards, the page says so instead of showing a number.

It is a reference, not a specification. For anything structural, pressure-bearing or safety-critical, check it against your drawing and your tap maker's own chart.