# Tap Drill Size Chart: Metric (M) and UNC/UNF

> Tap drill sizes for metric M1.6–M48 and UNC/UNF threads, with the D−P formula for 75% thread engagement and steel vs aluminum rules, per ISO 2306 / ASME B1.1.

https://www.sinbo-machining.com/wiki/reference/thread-tap-drill-sizes/

---

## On This Page

- The 75% Thread Rule (and the Formula Behind It)
- Metric Coarse (M) Tap Drill Sizes
- Metric Fine (MF) Tap Drill Sizes
- Inch UNC (Coarse) and UNF (Fine) Tap Drill Sizes
- Steel vs Aluminum vs Brass — When to Go Bigger
- Blind Holes, Through Holes, and Depth Rules
- Standards & Sources
- Common Mistakes
- Need threaded holes that don't strip or break taps?

# Tap Drill Size Chart — Metric and UNC/UNF
Pick the right pilot drill before tapping and you save a broken tap, a scrapped part, and a late-night call from the shop floor. Tables below cover metric M1.6–M48 and inch UNC/UNF #0 to 1 inch, at 75% thread engagement — the production default.
## The 75% Thread Rule (and the Formula Behind It)
Production tapping targets ~75% thread engagement, not 100%. A 100% thread demands ~3× the tapping torque of a 50% thread, and the extra strength of a full thread is rarely usable — the screw itself will fail first in almost any real joint. 75% is the sweet spot that ISO 2306 and ASME B1.1 both default to in their published tables. Metric (M threads): Tap Drill (mm) = Major Diameter − PitchInch (UNC/UNF): Tap Drill (inch) = Major Diameter − 1 / TPIBoth formulas give approximately 75% thread engagement. Tap-drill charts are just this formula pre-computed and rounded to a standard drill size. Why not 100%? Tapping torque rises steeply with thread engagement. Going from 50% to 100% engagement roughly triples the torque and doubles the risk of tap breakage — while adding only marginal pull-out strength, because the fastener’s tensile strength usually fails before the threads do.
## Metric Coarse (M) Tap Drill Sizes
Standard ISO metric coarse threads. Tap drill sizes per ISO 2306:1972 (still current for these sizes), cross-checked against ISO 724:2023 thread profiles and manufacturer tables.
|  Thread |  Pitch (mm) |  Tap Drill (mm) |  Closest inch drill |  % Thread (approx.)
|  M1.6 × 0.35 |  0.35 |  1.25 |  0.0490 in (#56) |  75%
|  M2 × 0.4 |  0.40 |  1.60 |  0.0629 in (#52) |  75%
|  M2.5 × 0.45 |  0.45 |  2.05 |  0.0807 in (#46) |  75%
|  M3 × 0.5 |  0.50 |  2.50 |  0.0984 in (#39) |  75%
|  M3.5 × 0.6 |  0.60 |  2.90 |  0.1142 in (#33) |  75%
|  M4 × 0.7 |  0.70 |  3.30 |  0.1299 in (#30) |  75%
|  M5 × 0.8 |  0.80 |  4.20 |  0.1654 in (#19) |  75%
|  M6 × 1.0 |  1.00 |  5.00 |  0.1969 in (#9) |  75%
|  M7 × 1.0 |  1.00 |  6.00 |  0.2362 in (15/64) |  75%
|  M8 × 1.25 |  1.25 |  6.80 |  0.2677 in (H) |  74%
|  M10 × 1.5 |  1.50 |  8.50 |  0.3346 in (Q) |  75%
|  M12 × 1.75 |  1.75 |  10.20 |  0.4016 in (Y) |  74%
|  M14 × 2.0 |  2.00 |  12.00 |  0.4724 in (31/64) |  75%
|  M16 × 2.0 |  2.00 |  14.00 |  0.5512 in (35/64) |  75%
|  M20 × 2.5 |  2.50 |  17.50 |  0.6890 in (11/16) |  74%
|  M24 × 3.0 |  3.00 |  21.00 |  0.8268 in (53/64) |  75%
|  M30 × 3.5 |  3.50 |  26.50 |  1.0433 in |  74%
|  M36 × 4.0 |  4.00 |  32.00 |  1.2598 in |  75%
|  M42 × 4.5 |  4.50 |  37.50 |  1.4764 in |  74%
|  M48 × 5.0 |  5.00 |  43.00 |  1.6929 in |  75%
Values in bold (M6, M8) are the most-used sizes in CNC machining — if you only memorize two, make it those.
## Metric Fine (MF) Tap Drill Sizes
Fine-pitch metric threads are used where vibration loosening is a concern, or where wall thickness limits thread depth. The same D − P formula applies.
|  Thread |  Pitch (mm) |  Tap Drill (mm) |  Typical use
|  M6 × 0.75 |  0.75 |  5.25 |  Thin-wall, fine adjustment
|  M8 × 1.0 |  1.00 |  7.00 |  Automotive, aerospace
|  M10 × 1.25 |  1.25 |  8.80 |  Aerospace fittings
|  M12 × 1.5 |  1.50 |  10.50 |  Hydraulic fittings, instruments
|  M14 × 1.5 |  1.50 |  12.50 |  Spark plug threads (some)
|  M16 × 1.5 |  1.50 |  14.50 |  Aerospace, automotive
|  M20 × 1.5 |  1.50 |  18.50 |  Hydraulic, instruments
|  M24 × 2.0 |  2.00 |  22.00 |  Heavy machinery, hydraulics

## Inch UNC (Coarse) and UNF (Fine) Tap Drill Sizes
Inch-series tap drills per ASME B1.1-2019, at 75% thread engagement. Drill sizes use the US number/letter/fraction system (a #36 drill is 0.1065 in; an F drill is 0.2570 in).
|  Thread |  TPI |  Major dia. (in) |  Tap Drill |  Tap Drill (in) |  Tap Drill (mm)
|  #0–80 UNF |  80 |  0.0600 |  3/64 |  0.0469 |  1.19
|  #1–64 UNC |  64 |  0.0730 |  #54 |  0.0550 |  1.40
|  #2–56 UNC |  56 |  0.0860 |  #50 |  0.0700 |  1.78
|  #3–48 UNC |  48 |  0.0990 |  #47 |  0.0785 |  1.99
|  #4–40 UNC |  40 |  0.1120 |  #43 |  0.0890 |  2.26
|  #5–40 UNC |  40 |  0.1250 |  #38 |  0.1015 |  2.58
|  #6–32 UNC |  32 |  0.1380 |  #36 |  0.1065 |  2.71
|  #8–32 UNC |  32 |  0.1640 |  #29 |  0.1360 |  3.45
|  #10–24 UNC |  24 |  0.1900 |  #25 |  0.1495 |  3.80
|  #10–32 UNF |  32 |  0.1900 |  #21 |  0.1590 |  4.04
|  1/4–20 UNC |  20 |  0.2500 |  #7 |  0.2010 |  5.11
|  1/4–28 UNF |  28 |  0.2500 |  #3 |  0.2130 |  5.41
|  5/16–18 UNC |  18 |  0.3125 |  F |  0.2570 |  6.53
|  5/16–24 UNF |  24 |  0.3125 |  I |  0.2720 |  6.91
|  3/8–16 UNC |  16 |  0.3750 |  5/16 |  0.3125 |  7.94
|  3/8–24 UNF |  24 |  0.3750 |  Q |  0.3320 |  8.43
|  7/16–14 UNC |  14 |  0.4375 |  U |  0.3680 |  9.35
|  1/2–13 UNC |  13 |  0.5000 |  27/64 |  0.4219 |  10.72
|  1/2–20 UNF |  20 |  0.5000 |  29/64 |  0.4531 |  11.51
|  5/8–11 UNC |  11 |  0.6250 |  17/32 |  0.5313 |  13.49
|  3/4–10 UNC |  10 |  0.7500 |  21/32 |  0.6563 |  16.67
|  7/8–9 UNC |  9 |  0.8750 |  49/64 |  0.7656 |  19.45
|  1–8 UNC |  8 |  1.0000 |  7/8 |  0.8750 |  22.23
The #6–32, #10–32, and 1/4–20 rows are bolded because they are the three most-used inch sizes in CNC machining for electronic and instrument housings.
## Steel vs Aluminum vs Brass — When to Go Bigger
The 75% tables above are the production default for steel, stainless, and titanium. For softer materials, you can drop the engagement — and many shops do, to reduce tap breakage:
|  Material |  Recommended engagement |  Why
|  Steel, stainless, titanium |  75% |  Standard. Strong threads, manageable tapping torque.
|  Aluminum (6061, 7075) |  65–70% |  Softer material; full threads strip before the screw anyway. Lower torque = less tap breakage.
|  Brass, copper |  60–65% |  Soft; galls; taps bind at high engagement.
|  Plastics (POM, PC, PEEK) |  55–65% |  Plastic threads fail by shear; lower engagement reduces tap breakage on glass-filled grades.
|  Thin wall (<1× diameter) |  Always reduce |  A thin wall physically cannot support a 75% thread; you’ll break through.
For lower engagement, increase the tap drill by: Δd = 0.0130 × P / engagement_fractionPer ASME B1.1 Appendix. For 70% engagement on M6×1.0: Δd = 0.0130 × 1.0 / 0.70 ≈ 0.019 mm — in practice, round up to the next standard drill (5.10 mm or #9).
## Blind Holes, Through Holes, and Depth Rules
The tap-drill diameter is only half the spec. The hole depth matters too:
|  Hole type |  Drill depth |  Thread depth (min) |  Notes
|  Through hole |  Through the part |  1.0–1.5× diameter |  Tap can clear chips out the back. Easiest to tap.
|  Blind hole, normal |  Thread depth + 0.5× D + lead |  1.0–1.5× D |  Drill 0.5× diameter deeper than threads to give chips room.
|  Blind hole, tough material |  Thread depth + 1.0× D + lead |  1.5× D |  Stainless / titanium; chips pack tighter.
|  Blind hole, spiral-point tap |  Thread depth + 1.0× D |  As above |  Spiral-point taps push chips ahead; need chip room below.
Effective thread length ≠ drill depth. The first thread (lead) and the last thread (incomplete) don’t count. In a blind hole, only ~80% of the tapped length carries load. Always specify thread engagement length on drawings, not total hole depth.
## Standards & Sources
Primary standardsISO 2306:1972 Solid tapping drill sizes for use in conjunction with ISO metric screw threads (still current for the sizes in this page; values re-validated by later ISO 2306 technical reports).ISO 724:2023 Metric ISO screw threads — Basic dimensions (thread profile; used to compute tap drill from D−P).ASME B1.1-2019 Unified Inch Screw Threads, UN and UNR Thread Form. Defines the inch-series tap-drill tables and the 75% engagement formula. Related thread standardsISO 261 Metric screw threads — General plan · ISO 965 Metric thread tolerances · ASME B1.13M Metric screw threads—M profile (the metric counterpart to ASME B1.1).
## Common Mistakes

|  # |  Mistake |  What goes wrong |  Fix
|  1 |  Specifying 100% thread engagement |  3× tapping torque, frequent tap breakage, marginal strength gain |  Use 75% (the standard tables). Drop to 60–70% for soft materials.
|  2 |  Using a drill bit that’s “close enough” |  Engagement changes by 10–15%, either stripping threads or breaking taps |  Use the exact drill from the table; if you don’t have it, go to the next larger size and accept lower engagement.
|  3 |  Drilling exactly to thread depth |  Tap lead chatters; bottom threads incomplete; chips pack |  Drill 0.5×D deeper than required thread depth (1.0×D for tough materials).
|  4 |  Treating fine pitch like coarse |  Fine pitch needs a smaller drill (by D−P), and a more rigid setup to avoid cross-threading |  Always check pitch. Fine pitch on a thin wall often needs a thicker wall or a helicoil.
|  5 |  Tapping too fast in stainless or titanium |  Tap welds itself into the hole and snaps |  Drop RPM to 1/3 of steel; use spiral-flute tap; use high-sulfur tapping fluid.
|  6 |  Specifying the thread callout without pitch |  “M10” is ambiguous — could be 1.5 coarse or 1.25 fine, drills differ by 0.3 mm |  Always specify full callout: M10×1.5–6H or 1/4–20 UNC–2B.
|  7 |  Reaming the tap-drill hole first |  Reamed hole has no clearance for chips; tap breaks |  Tap drills are intentionally a bit rough; don’t ream. Ream only the clearance hole if a separate clearance hole is needed.
Frequently Asked Questions What size drill do I use for an M6 × 1.0 thread? 5.0 mm (a #9 inch drill at 0.1969 in also works). This is the most-used metric tap-drill size in CNC machining. The simple rule: tap drill = major diameter − pitch, so 6 − 1 = 5 mm. What is the 75% thread engagement rule? Production tapping targets roughly 75% thread engagement — meaning the tap drill is sized so only 75% of the thread profile is cut. Going higher (toward 100%) triples the tapping torque and dramatically raises tap-breakage risk, while adding almost no usable strength because the fastener fails first. The 75% level is what ISO 2306 and ASME B1.1 default to in their standard tables. Why is the formula different for metric vs inch threads? It isn’t — both are the same idea. For metric, you subtract the pitch (e.g. 1.0 mm for M6). For inch, you subtract 1/TPI (e.g. 1/20 = 0.050 in for 1/4–20). In both cases: tap_drill = major_diameter − thread_pitch, where pitch is the distance per thread. Should I reduce thread engagement in aluminum? Often yes. In soft materials like 6061-T6 aluminum, brass, and most plastics, a 65–70% engagement gives you essentially the same strength as 75% with much lower tapping torque and lower tap-breakage risk. For thin walls (less than 1× diameter), you may need to drop further or switch to a helicoil. Can I use a 100% thread for stronger joints? Almost never worth it. The fastener’s tensile strength is usually the limiting factor, not the thread pull-out. A 100% thread engagement roughly triples tapping torque and risks breaking the tap (which then has to be extracted from your part, often scrapping it). The marginal extra strength is rarely usable. If the joint really needs more strength, use a larger screw or a longer engagement length, not a deeper thread profile. How much deeper than the thread should I drill a blind hole? Add at least 0.5× the major diameter beyond the required thread length for chip clearance. For tough materials (stainless, titanium, Inconel), make that 1.0× diameter. The first thread (lead) and the last thread (incomplete) don’t carry load — only ~80% of the tapped length is fully engaged. What drill bit is a #7 or an F drill? US number-and-letter drill sizes: #7 = 0.2010 in (5.11 mm), used for 1/4–20 UNC. F = 0.2570 in (6.53 mm), used for 5/16–18 UNC. The full number series runs #80 (0.0135 in) to #1 (0.2280 in); the letter series runs A (0.2340 in) to Z (0.4130 in). Beyond Z, drills are specified as fractions of an inch. Sources & Standards Referenced 1- ISO 2306:1972: Solid tapping drill sizes for use in conjunction with ISO metric screw threads
1- ISO 724:2023: Metric ISO screw threads — Basic dimensions (thread profile and D−P derivation)
1- ISO 261:1998: General purpose metric screw threads — General plan
1- ASME B1.1-2019: Unified Inch Screw Threads, UN and UNR Thread Form (inch tap-drill tables and engagement formula)
1- ASME B1.13M-2018: Metric screw threads — M profile
1- Machinery's Handbook 31st Edition (Industrial Press, 2020), Tap Drill Sizes section

## Need threaded holes that don't strip or break taps?
We tap thousands of M-series and UNC/UNF holes a month across steel, stainless, aluminum, titanium, and plastic. Send your drawing and we'll quote in 24 hours. [Request a Quote ](https://www.sinbo-machining.com/quote/)