Machining Reference · Thread Prep
Tap Drill Size Chart — Metric and Imperial (UNC / UNF)
Every tap needs a hole of a specific diameter before it cuts, and that diameter is not the thread size printed on the tap. This page gives the tap drill size for ISO metric coarse and fine threads from M1.6 to M20 and for UNC and UNF threads from #0 to 1 inch, shows the arithmetic behind each number so you can size a thread that is not on the chart, and explains when to move one drill size up. Asking for the bit size for a 1/4 20 tap — 0.201 in, a #7 drill — is the most common single question we get from workshops, so the table is built to answer that class of question in one line.
- Metric coarse and fine, M1.6 – M20 (ISO 261 pitches)
- UNC and UNF, #0 – 1 in (ASME B1.1-2024 thread data)
- Stocked drill diameter and the thread engagement it actually leaves
- Rule of thumb: metric tap drill = major diameter minus pitch
- Higher engagement for soft material, lower for stainless and titanium
- Print-friendly tables — no script needed to read them
Sources: drill diameter series ASME B94.11M-1993 (Twist Drills, stabilized maintenance) · thread dimensions ASME B1.1-2024 (Unified Inch Screw Threads) and ISO 261 (ISO general purpose metric screw threads) · tap drill diameters ISO 2306:1972 (Drills for use prior to tapping screw threads, drill diameter approximately equal to nominal thread diameter minus pitch) · engagement percentages computed with drill = D − 1.29904 × P × engagement (60° thread form, 75% target). Every stocked drill in the tables was cross-checked row by row against published tap drill charts; the small deviations that stocked diameters create are visible in the engagement column rather than hidden.
Full Tap Drill Tables
Tap drill sizes for metric M1.6 to M20 and UNC / UNF #0 to 1 inch
Two groups below. The metric table covers the coarse series every drawing starts from plus the fine pitches that appear on thin-wall parts and adjustment threads. The imperial table covers UNC and UNF in both the number sizes below 1/4 in and the fractional sizes from 1/4 in upward. Each row gives the thread callout, the pitch, the nominal tap drill from the major-diameter-minus-pitch rule, the stocked drill you can order, and the thread engagement that stocked drill leaves — because those last two are not always the same number, and the gap is exactly what a shop needs to know before tapping stainless.
ISO metric threads — coarse and fine pitch
| Thread | Pitch (mm) | Series | Major minus pitch (mm) | Tap drill, stocked (mm) | Engagement |
|---|---|---|---|---|---|
| M1.6 × 0.35 | 0.35 | Coarse | 1.25 | 1.25 | 77.0% |
| M2 × 0.4 | 0.4 | Coarse | 1.6 | 1.6 | 77.0% |
| M2.5 × 0.45 | 0.45 | Coarse | 2.05 | 2.05 | 77.0% |
| M3 × 0.5 | 0.5 | Coarse | 2.5 | 2.5 | 77.0% |
| M3.5 × 0.6 | 0.6 | Coarse | 2.9 | 2.9 | 77.0% |
| M4 × 0.7 | 0.7 | Coarse | 3.3 | 3.3 | 77.0% |
| M5 × 0.8 | 0.8 | Coarse | 4.2 | 4.2 | 77.0% |
| M6 × 1 | 1 | Coarse | 5 | 5 | 77.0% |
| M7 × 1 | 1 | Coarse | 6 | 6 | 77.0% |
| M8 × 1.25 | 1.25 | Coarse | 6.75 | 6.8 | 73.9% |
| M10 × 1.5 | 1.5 | Coarse | 8.5 | 8.5 | 77.0% |
| M12 × 1.75 | 1.75 | Coarse | 10.25 | 10.2 | 79.2% |
| M14 × 2 | 2 | Coarse | 12 | 12 | 77.0% |
| M16 × 2 | 2 | Coarse | 14 | 14 | 77.0% |
| M18 × 2.5 | 2.5 | Coarse | 15.5 | 15.5 | 77.0% |
| M20 × 2.5 | 2.5 | Coarse | 17.5 | 17.5 | 77.0% |
| M8 × 1 | 1 | Fine | 7 | 7 | 77.0% |
| M10 × 1.25 | 1.25 | Fine | 8.75 | 8.8 | 73.9% |
| M10 × 1 | 1 | Fine | 9 | 9 | 77.0% |
| M12 × 1.5 | 1.5 | Fine | 10.5 | 10.5 | 77.0% |
| M12 × 1.25 | 1.25 | Fine | 10.75 | 10.8 | 73.9% |
| M14 × 1.5 | 1.5 | Fine | 12.5 | 12.5 | 77.0% |
| M16 × 1.5 | 1.5 | Fine | 14.5 | 14.5 | 77.0% |
| M18 × 1.5 | 1.5 | Fine | 16.5 | 16.5 | 77.0% |
| M20 × 1.5 | 1.5 | Fine | 18.5 | 18.5 | 77.0% |
Metric drill diameters follow ISO 2306:1972, where the drill diameter is approximately the nominal thread diameter minus the pitch, and the stocked sizes are the millimetre drills a supplier actually keeps on the shelf (ISO 235 series). Where the two differ — M8 × 1.25 computes to 6.75 mm and ships as 6.8 mm, M12 × 1.75 computes to 10.25 mm and ships as 10.2 mm — the stocked column is what you order and the engagement column shows what it leaves.
UNC and UNF threads — #0 to 1 inch
| Thread size | Series | Threads per inch | Tap drill | Drill diameter (in) | Drill diameter (mm) | Engagement |
|---|---|---|---|---|---|---|
| #0 · 80 | UNF | 80 | 3/64 | 0.0469 | 1.191 | 80.8% |
| #1 · 64 | UNC | 64 | #53 | 0.0595 | 1.511 | 66.5% |
| #1 · 72 | UNF | 72 | #53 | 0.0595 | 1.511 | 74.8% |
| #2 · 56 | UNC | 56 | #50 | 0.07 | 1.778 | 69.0% |
| #2 · 64 | UNF | 64 | #50 | 0.07 | 1.778 | 78.8% |
| #3 · 48 | UNC | 48 | #47 | 0.0785 | 1.994 | 75.7% |
| #3 · 56 | UNF | 56 | #45 | 0.082 | 2.083 | 73.3% |
| #4 · 40 | UNC | 40 | #43 | 0.089 | 2.261 | 70.8% |
| #4 · 48 | UNF | 48 | #42 | 0.0935 | 2.375 | 68.4% |
| #5 · 40 | UNC | 40 | #38 | 0.1015 | 2.578 | 72.4% |
| #5 · 44 | UNF | 44 | #37 | 0.104 | 2.642 | 71.1% |
| #6 · 32 | UNC | 32 | #36 | 0.1065 | 2.705 | 77.6% |
| #6 · 40 | UNF | 40 | #33 | 0.113 | 2.87 | 77.0% |
| #8 · 32 | UNC | 32 | #29 | 0.136 | 3.454 | 69.0% |
| #8 · 36 | UNF | 36 | #29 | 0.136 | 3.454 | 77.6% |
| #10 · 24 | UNC | 24 | #25 | 0.1495 | 3.797 | 74.8% |
| #10 · 32 | UNF | 32 | #21 | 0.159 | 4.039 | 76.4% |
| #12 · 24 | UNC | 24 | #16 | 0.177 | 4.496 | 72.1% |
| #12 · 28 | UNF | 28 | #14 | 0.182 | 4.623 | 73.3% |
| 1/4" · 20 | UNC | 20 | #7 | 0.201 | 5.105 | 75.4% |
| 1/4" · 28 | UNF | 28 | #3 | 0.213 | 5.41 | 79.8% |
| 5/16" · 18 | UNC | 18 | F | 0.257 | 6.528 | 76.9% |
| 5/16" · 24 | UNF | 24 | I | 0.272 | 6.909 | 74.8% |
| 3/8" · 16 | UNC | 16 | 5/16 | 0.3125 | 7.938 | 77.0% |
| 3/8" · 24 | UNF | 24 | Q | 0.332 | 8.433 | 79.4% |
| 7/16" · 14 | UNC | 14 | U | 0.368 | 9.347 | 74.9% |
| 7/16" · 20 | UNF | 20 | 25/64 | 0.3906 | 9.922 | 72.2% |
| 1/2" · 13 | UNC | 13 | 27/64 | 0.4219 | 10.716 | 78.2% |
| 1/2" · 20 | UNF | 20 | 29/64 | 0.4531 | 11.509 | 72.2% |
| 5/8" · 11 | UNC | 11 | 17/32 | 0.5312 | 13.494 | 79.4% |
| 5/8" · 18 | UNF | 18 | 9/16 | 0.5625 | 14.287 | 86.6% |
| 3/4" · 10 | UNC | 10 | 21/32 | 0.6562 | 16.669 | 72.2% |
| 3/4" · 16 | UNF | 16 | 11/16 | 0.6875 | 17.462 | 77.0% |
| 7/8" · 9 | UNC | 9 | 25/32 | 0.7812 | 19.844 | 65.0% |
| 7/8" · 14 | UNF | 14 | 13/16 | 0.8125 | 20.637 | 67.4% |
| 1" · 8 | UNC | 8 | 7/8 | 0.875 | 22.225 | 77.0% |
| 1" · 12 | UNF | 12 | 29/32 | 0.9062 | 23.019 | 86.6% |
Inch drill designations are the three overlapping series of ASME B94.11M-1993: fractional drills stepping in 1/64 in, number drills from #80 up to #1, and letter drills A to Z filling the range just above 1/4 in. Thread data — major diameter and threads per inch for both the coarse and fine series — comes from ASME B1.1-2024. Rows above 1/2 in are marked by their engagement value: 5/8-18 and 1-12 land near 87% with a stocked fraction, which is tight for stainless, so the one-size-up rule in the next section matters most there.
How to Use the Chart
Three steps from a thread callout to a drilled hole
1. Read the thread callout, not the bolt size
A callout such as 1/4-20 UNC or M10 × 1.5 carries two facts you need: the nominal diameter and the pitch, either as threads per inch (20) or as a pitch in millimetres (1.5). A bolt described only as M10 is coarse by default — M10 × 1.5 — but the same diameter in fine is M10 × 1.25. Take the pitch from the drawing or measure it: coarse and fine of the same diameter need different drills, and using the coarse drill for a fine thread leaves the hole undersized enough to bind and break the tap.
2. Find the row, then confirm the stocked drill
Read across the row: the nominal figure comes from the standard, and the stocked drill is the nearest drill that a supplier stocks. For metric threads that is a millimetre size in the ISO 235 series; for inch threads it is a fractional, number or letter drill from ASME B94.11M-1993. When the two are not identical the engagement column tells you which way you have moved — 6.8 mm on M8 × 1.25 leaves 73.9% rather than the 75% the formula targets, which is a safe direction to be off in. If you are working across unit systems, 1 in = 25.4 mm exactly: a #7 drill is 0.2010 in or 5.105 mm, and a 6.8 mm drill is 0.2677 in, close to a 17/64 in drill for anyone without metric sizes.
3. Adjust for material, depth and tap type
The chart is a general-shop baseline for cutting taps in steel and aluminum. Stainless, titanium, high-nickel alloys and deep blind holes want one size larger — around 60-65% engagement — to cut tapping torque. Forming taps need their own, larger drill from the tap supplier. Blind holes need the drilled depth to exceed the thread depth by the tap chamfer plus a few threads of chip room, and a small countersink at the mouth keeps the first thread from tearing. And whatever the calculation says, the tap maker chart for the exact tap wins on a critical part.
The arithmetic, if the thread is not on the chart
- Metric: tap drill = major diameter − pitch. M12 × 1.75 → 12 − 1.75 = 10.25 mm, ordered as 10.2 mm.
- Inch, 75% engagement: tap drill = major diameter − (1.29904 × 0.75 ÷ threads per inch). 1/4-20 → 0.250 − (0.9743 ÷ 20) = 0.201 in = #7.
- Engagement actually produced: % = (major diameter − drill) × threads per inch ÷ 1.29904 × 100.
- Blank diameter for forming taps: take from the tap supplier data — not from this column.
Common lookups
- 1/4-20 UNC — #7, 0.2010 in / 5.105 mm
- 5/16-18 UNC — F, 0.2570 in / 6.528 mm
- 3/8-16 UNC — 5/16 in, 0.3125 in / 7.938 mm
- 1/2-13 UNC — 27/64 in, 0.4219 in / 10.716 mm
- M6 × 1 — 5.0 mm
- M8 × 1.25 — 6.8 mm
- M10 × 1.5 — 8.5 mm
- M12 × 1.75 — 10.2 mm
These are the rows the table is asked for most often in quotations. The full set is in the table above — this list repeats nothing that is not already there.
Machining Reference Tools
Related calculation and conversion tools
Thread preparation is one leg of the arithmetic a workshop repeats every week. The other two references on this page's tool row cover what happens around it: hardness conversion tells you which drill grade and tap coating the workpiece calls for, and the cutting speed calculator turns a recommended surface speed into the rpm your machine can actually be set to.
Read together, the three pages answer the same three questions every tapping job starts with — what hole, what material condition, and what speed.
Hardness
Hardness Conversion Chart
HRC, HB, HV and tensile strength conversion for steel — so the drill grade you order matches the material you are tapping.
Open toolCutting Data
Cutting Speed Calculator
Turn a recommended surface speed into spindle rpm for any drill or tap diameter, metric or inch.
Open toolCatalogue
Drill Bits and Drilling Tools
Solid carbide, HSS jobber and indexable drills sized to the hole you just calculated — 1 to 60 mm.
Open toolBuy the Right Tool
Once the hole is sized, the drill and the tap have to match each other
The three ranges below are the ones this chart sends people to. Taps and threading tools cover the cutting side of the thread — straight flute, spiral point and spiral flute series in metric and UNC, plus forming taps for chipless threads. Drill bits cover the hole, from solid carbide twist drills to HSS jobber and indexable U-drills as the diameter grows. Holders and collets cover the part most often forgotten until a tap snaps: keeping the tap square to the drilled hole, so the thread starts straight and gauges clean.
A correct hole size only gets you as far as the pilot. What decides whether the thread comes out to gauge is the pair either side of it: the drill that made the hole and the tap that cuts into it. A drill that has been reground oversize, or a coated drill ordered in the wrong class, moves the hole outside the tolerance the tap expects — and the tap is usually blamed for a problem that started at the drill.
We supply the pair. Send the thread callout, the material, the thread depth and whether the hole is through or blind, and we come back with the drill (carbide or HSS, coated for the material), the tap type that suits the hole — straight flute for through holes, spiral flute for blind, forming for chipless threads — the holders and collets that keep the tap square, and a starting speed and feed for the combination. Trial quantities and mixed orders are normal: a workshop ordering six taps and six matching drills in one thread size is the case this page exists for.
For anything outside the tables — M22 and above, UNEF, NPT and BSP pipe threads, non-standard pitches, or a print that specifies a tolerance class rather than a drill — send the drawing and we will confirm the size against the standard before quoting.
Threading
Taps and Threading Tools
Straight flute, spiral point, spiral flute and forming taps, plus thread mills — metric and UNC/UNF.
See the rangeDrilling
Drill Bits for Metal
Carbide twist drills to DIN 6537 and 6539, HSS jobber to DIN 338, and indexable U-drills for larger holes.
See the rangeWorkholding
Tap Holders and Collets
Tension-compression tap holders and collet chucks that keep the tap square to the drilled hole.
See the rangeQuestions Buyers Ask
Reading the chart, thread engagement and out-of-chart sizes
A #7 drill, 0.201 in (5.105 mm), for about 75% thread engagement. In fractional terms it sits between 13/64 and 7/32, which is why the number series exists. The metric equivalent in the table is 5.1 mm if your shop works in metric only.
A tap does not cut a hole, it cuts a thread into the wall of a hole that is already there. The hole must be smaller than the thread major diameter and larger than the thread minor diameter, so the tap has material to remove on both sides. Size it too small and the tap is overloaded and may snap; size it too large and the thread is shallow and strips under load.
Going from 75% to 100% engagement adds roughly 5% to the strength of the thread but about three times the tapping torque, and the extra load is what breaks taps, particularly in the small sizes. Published charts, including the ISO 2306 drill sizes used here, are built around a normal engagement close to 75%, and the stocked drill you can actually buy lands between about 65% and 87%.
Stainless steel, titanium, high-nickel alloys and any material that work-hardens. Moving one drill size above the chart value drops engagement toward 60-65%, which cuts tapping torque and tap breakage sharply while keeping almost all of the thread strength. Aluminum, brass and free-cutting steel run happily at the chart figure, and very thin or soft sections can go up to 80% or so for extra grip.
No. Forming (roll) taps displace material instead of cutting it, so they need a larger hole than the cutting tap in this chart — the tap maker publishes a dedicated drill size for each forming tap, usually close to the thread pitch diameter rather than this table value. Treat the chart on this page as the cutting-tap reference and take forming tap sizes from the tap supplier data.
No. The three groups have different thread forms and pitch conventions: ISO metric uses a pitch in millimetres, UN and UNF use threads per inch, and pipe threads are specified by nominal bore with their own tables. Mixing them is how an undersized hole gets drilled. If your drawing calls for a thread that is not on this page, send the thread callout and material and we will confirm the drill against the standard.
The thread and drill dimensions come from the standards named above, and the engagement column shows exactly what each stocked diameter leaves, so any difference between charts is visible rather than hidden. For a critical hole the tap maker chart for that specific tap and tolerance class wins, because it accounts for the tap geometry and the gauge system; treat this page as the general-shop reference.
Every row here comes from one formula, so you can size anything: metric, subtract the pitch from the major diameter; inch, subtract 1.29904 × 0.75 ÷ threads per inch from the major diameter, then pick the nearest standard drill below. For sizes outside the table — M22 and above, UNEF, pipe threads, or a non-standard pitch — send us the callout, material and thread depth and we reply with the drill, the tap type and starting cutting data.
Get your tap drill, tap and holder quoted as one set
Send the thread callout, the material and whether the hole is through or blind — you get the tap type, the matching drill, the holders and a starting speed and feed, not a catalogue.