Tap drill size calculator.
The tap drill for any thread and engagement, with the nearest inch and metric drills and the engagement each one gives.
Pick a thread
Tap drill sizes at 75% engagement
This chart lists every thread in the calculator at 75%, worked out by the same formula, with the nearest standard drill in each system and the engagement that drill gives. Where the inch and metric drills give noticeably different engagement, it is worth comparing both before you pick one.
| Thread | Major dia. | Pitch / TPI | Theoretical | Inch drill | Gives | Metric drill | Gives |
|---|---|---|---|---|---|---|---|
| #0-80 UNF | 0.0600" | 80 TPI | 0.0478" | 3/64" | 81% | 1.2 mm | 79% |
| #1-64 UNC | 0.0730" | 64 TPI | 0.0578" | #53 | 67% | 1.5 mm | 69% |
| #1-72 UNF | 0.0730" | 72 TPI | 0.0595" | #53 | 75% | 1.5 mm | 77% |
| #2-56 UNC | 0.0860" | 56 TPI | 0.0686" | #50 | 69% | 1.7 mm | 82% |
| #2-64 UNF | 0.0860" | 64 TPI | 0.0708" | #50 | 79% | 1.8 mm | 75% |
| #3-48 UNC | 0.0990" | 48 TPI | 0.0787" | #47 | 76% | 2 mm | 75% |
| #3-56 UNF | 0.0990" | 56 TPI | 0.0816" | #45 | 73% | 2.1 mm | 70% |
| #4-40 UNC | 0.1120" | 40 TPI | 0.0876" | #43 | 71% | 2.2 mm | 78% |
| #4-48 UNF | 0.1120" | 48 TPI | 0.0917" | #42 | 68% | 2.3 mm | 79% |
| #5-40 UNC | 0.1250" | 40 TPI | 0.1006" | #38 | 72% | 2.6 mm | 70% |
| #5-44 UNF | 0.1250" | 44 TPI | 0.1029" | #37 | 71% | 2.6 mm | 77% |
| #6-32 UNC | 0.1380" | 32 TPI | 0.1076" | #36 | 78% | 2.7 mm | 78% |
| #6-40 UNF | 0.1380" | 40 TPI | 0.1136" | #33 | 77% | 2.9 mm | 73% |
| #8-32 UNC | 0.1640" | 32 TPI | 0.1336" | #29 | 69% | 3.4 mm | 74% |
| #8-36 UNF | 0.1640" | 36 TPI | 0.1369" | #29 | 78% | 3.5 mm | 73% |
| #10-24 UNC | 0.1900" | 24 TPI | 0.1494" | #25 | 75% | 3.8 mm | 75% |
| #10-32 UNF | 0.1900" | 32 TPI | 0.1596" | #21 | 76% | 4 mm | 80% |
| #12-24 UNC | 0.2160" | 24 TPI | 0.1754" | #16 | 72% | 4.5 mm | 72% |
| #12-28 UNF | 0.2160" | 28 TPI | 0.1812" | #14 | 73% | 4.5 mm | 84% |
| 1/4-20 UNC | 0.2500" | 20 TPI | 0.2013" | #7 | 75% | 5.2 mm | 70% |
| 1/4-28 UNF | 0.2500" | 28 TPI | 0.2152" | #3 | 80% | 5.5 mm | 72% |
| 5/16-18 UNC | 0.3125" | 18 TPI | 0.2584" | F | 77% | 6.5 mm | 78% |
| 5/16-24 UNF | 0.3125" | 24 TPI | 0.2719" | I | 75% | 7 mm | 68% |
| 3/8-16 UNC | 0.3750" | 16 TPI | 0.3141" | 5/16" | 77% | 8 mm | 74% |
| 3/8-24 UNF | 0.3750" | 24 TPI | 0.3344" | Q | 79% | 8.5 mm | 75% |
| 7/16-14 UNC | 0.4375" | 14 TPI | 0.3679" | U | 75% | 9.2 mm | 81% |
| 7/16-20 UNF | 0.4375" | 20 TPI | 0.3888" | 25/64" | 72% | 9.8 mm | 80% |
| 1/2-13 UNC | 0.5000" | 13 TPI | 0.4251" | 27/64" | 78% | 11 mm | 67% |
| 1/2-20 UNF | 0.5000" | 20 TPI | 0.4513" | 29/64" | 72% | 11.5 mm | 73% |
| 9/16-12 UNC | 0.5625" | 12 TPI | 0.4813" | 31/64" | 72% | 12 mm | 83% |
| 9/16-18 UNF | 0.5625" | 18 TPI | 0.5084" | 33/64" | 65% | 13 mm | 70% |
| 5/8-11 UNC | 0.6250" | 11 TPI | 0.5364" | 17/32" | 79% | 13.5 mm | 79% |
| 5/8-18 UNF | 0.6250" | 18 TPI | 0.5709" | 37/64" | 65% | 14.5 mm | 75% |
| 3/4-10 UNC | 0.7500" | 10 TPI | 0.6526" | 21/32" | 72% | 17 mm | 62% |
| 3/4-16 UNF | 0.7500" | 16 TPI | 0.6891" | 11/16" | 77% | 18 mm | 51% |
| 7/8-9 UNC | 0.8750" | 9 TPI | 0.7668" | 49/64" | 76% | 19 mm | 88% |
| 7/8-14 UNF | 0.8750" | 14 TPI | 0.8054" | 13/16" | 67% | 20 mm | 94% |
| 1"-8 UNC | 1.0000" | 8 TPI | 0.8782" | 7/8" | 77% | 22 mm | 82% |
| 1"-12 UNF | 1.0000" | 12 TPI | 0.9188" | 59/64" | 72% | 22 mm | 124% |
| M2 x 0.4 | 2 mm | 0.4 mm | 1.61 mm | #52 | 74% | 1.6 mm | 77% |
| M2.5 x 0.45 | 2.5 mm | 0.45 mm | 2.06 mm | #46 | 76% | 2.1 mm | 68% |
| M3 x 0.5 | 3 mm | 0.5 mm | 2.51 mm | #39 | 73% | 2.5 mm | 77% |
| M4 x 0.7 | 4 mm | 0.7 mm | 3.32 mm | #30 | 81% | 3.3 mm | 77% |
| M5 x 0.8 | 5 mm | 0.8 mm | 4.22 mm | #19 | 75% | 4.2 mm | 77% |
| M6 x 1.0 | 6 mm | 1 mm | 5.03 mm | #8 | 73% | 5 mm | 77% |
| M8 x 1.25 | 8 mm | 1.25 mm | 6.78 mm | H | 77% | 6.8 mm | 74% |
| M8 x 1.0 | 8 mm | 1 mm | 7.03 mm | J | 74% | 7 mm | 77% |
| M10 x 1.5 | 10 mm | 1.5 mm | 8.54 mm | R | 71% | 8.5 mm | 77% |
| M10 x 1.25 | 10 mm | 1.25 mm | 8.78 mm | 11/32" | 78% | 8.8 mm | 74% |
| M12 x 1.75 | 12 mm | 1.75 mm | 10.30 mm | 13/32" | 74% | 10.5 mm | 66% |
| M12 x 1.25 | 12 mm | 1.25 mm | 10.78 mm | 27/64" | 79% | 11 mm | 62% |
| M14 x 2.0 | 14 mm | 2 mm | 12.05 mm | 15/32" | 81% | 12 mm | 77% |
| M16 x 2.0 | 16 mm | 2 mm | 14.05 mm | 35/64" | 81% | 14 mm | 77% |
| M16 x 1.5 | 16 mm | 1.5 mm | 14.54 mm | 37/64" | 68% | 14.5 mm | 77% |
| M20 x 2.5 | 20 mm | 2.5 mm | 17.56 mm | 11/16" | 78% | 18 mm | 62% |
| M24 x 3.0 | 24 mm | 3 mm | 21.08 mm | 53/64" | 76% | 21 mm | 77% |
Why 75% is a habit, and when to change it
Published charts assume 75%, and most shops never change it. The number came from general purpose work in mild materials, and it is a reasonable default there. It is a poor default in Inconel, in a deep blind hole, or anywhere a broken tap costs more than the part.
Two more things decide whether the hole is accepted. It has to sit where the drawing says, which is a positional tolerance separate from the size this page works out, and the positional check works from the same X and Y deviation an inspection report already carries. The drill also has to run at a speed the material tolerates, and starting surface speeds by material covers forty materials.
| Engagement | Where it belongs | The trade |
|---|---|---|
| 50% to 55% | Tough alloys, deep holes, machine tapping, thin taps | Substantially lower torque, very little strength given up |
| 60% to 65% | Stainless, titanium, production tapping | The usual production compromise |
| 70% to 75% | General work in aluminum, mild steel, brass | The chart default, and fine in free machining material |
| Above 80% | Rarely, and usually by accident | Torque rises sharply, strength barely moves, taps break |
Questions machinists ask about tap drills
How do you calculate tap drill size?
Subtract the thread depth you want from the major diameter. For a 60 degree unified or metric thread, the expression is: drill = major diameter minus (percentage of engagement times 1.299 times pitch, divided by 100), with pitch in the same units as the diameter. In inch practice, pitch is one divided by threads per inch, so the same formula is usually written as major diameter minus (percentage times 1.299) divided by (TPI times 100).
What percentage of thread engagement should I use?
Seventy five percent is the conventional default in general work, and it is what published tap drill charts assume. Going higher adds very little strength and a great deal of tapping torque, and that is how taps break. Fifty to sixty percent is common in tough alloys, in deep holes, and in anything tapped on a machine, because the strength you give up against a 75 percent thread is small and the torque you save is large.
Why does a higher percentage of thread not mean a stronger joint?
Once the engagement length is adequate, a properly engaged fastener fails in the bolt before the threads strip. Past about 60 percent, extra engagement mostly adds friction and tapping torque, with little gain in pull-out strength. Engagement length matters much more than engagement percentage: a 50 percent thread in a hole one and a half diameters deep is stronger than a 75 percent thread in a shallow one.
What is the tap drill for 1/4-20?
The tap drill for 1/4-20 is a #7 drill at 0.2010 inches. At 75 percent engagement the theoretical size is 0.2013 inches, and the #7 is the nearest standard drill. That gives 75 percent engagement in practice. The nearest metric drill is 5.2 mm, giving 70 percent.
Does this work for metric threads?
Yes, and the formula is the same one. For metric threads, pitch is stated directly in millimeters instead of as threads per inch, so the expression becomes major diameter minus (percentage times 1.299 times pitch) divided by 100. An M6 by 1.0 at 75 percent gives 5.03 mm, which is why the standard drill is 5.0 mm.
Should I use the same drill for a roll form tap?
No. Form tapping pushes material into shape instead of cutting it away, so the hole starts larger and the thread is raised into place. Roll form tap drills run close to 65 to 75 percent of the equivalent cut tap drill depth of engagement, and the correct size comes from the tap manufacturer. Using a cut tap drill with a form tap will usually break the tap.
Why do published charts sometimes disagree with the formula?
Published charts have to pick a drill that exists, and the formula gives a size that usually does not. The theoretical size for 3/8-16 at 75 percent is 0.3141 inches, which no standard drill matches exactly. A 5/16 inch drill gives 77 percent and an 8 mm drill gives 74 percent, and both are perfectly reasonable. A chart picks one without saying why, so this page shows the engagement each candidate actually produces.
Who made it, and what it does not do
This tool was written by Shopfloor Agency's lead engineer, who holds a bachelor’s degree in mechanical engineering and builds websites for US manufacturers. It runs entirely in your browser.
The formula is exact geometry for a 60 degree thread, and the chart is worked out from it directly. What it cannot know is your material, your tap, your hole depth, or whether you are cutting or forming the thread. Form taps need a different and larger hole from the tap manufacturer, and using a cut tap drill with one will usually break it.
If you spot an error, tell us, and we will correct the page and note the change.
We build websites for the shops that use tools like this.
We work only with US manufacturers and industrial service companies, so you never have to explain your trade. A website is a fixed $6,000, and the source code is yours at launch. Tell us what you make and who buys it, and we will reply with the scope and a delivery date.