Tap Drill Size Calculator
Calculate tap drill sizes for metric, UNC, UNF, and NPT threads. Pick the thread and tap type to see the exact hole diameter and closest standard drill.
Choose your thread
Series, size, and tap type.
Recommended tap drill
Calculated diameter, approximate drill, and reference dimensions.
Recommended tap drill
1.51 mm0.0595″- Alternate option
- #53
- Decimal diameter
- 0.0595"
- Close fit clearance
- #48
- Free fit clearance
- #46
Cutting tap sizes come from standard 75% tap drill charts—not a calculated decimal. Forming taps use divisor 175 (larger hole). Approximate drill rounds up to the next stocked size.
Upload your CAD for a quoteTap Drill Tables
Tap drill charts, screw clearance (close/free fit), and standard drill catalogs. All values in mm and inches.
| Thread | Examples | Major Ø | Tap Drills Ø | Drill |
|---|---|---|---|---|
| M1×0.25 | — | 1.00 mm0.0394″ | 0.75 mm0.0295″ | #69 |
| M1.2×0.25 | — | 1.20 mm0.0472″ | 0.95 mm0.0374″ | #63 |
| M1.4×0.3 | — | 1.40 mm0.0551″ | 1.10 mm0.0433″ | #57 |
| M1.6×0.35 | — | 1.60 mm0.063″ | 1.25 mm0.0492″ | 1.3 mm |
| M1.8×0.35 | — | 1.80 mm0.0709″ | 1.45 mm0.0571″ | 1.4 mm |
| M2×0.4 | — | 2.00 mm0.0787″ | 1.60 mm0.063″ | 4/64 |
| M2.5×0.45 | — | 2.50 mm0.0984″ | 2.05 mm0.0807″ | #46 |
| M3×0.5 | — | 3.00 mm0.1181″ | 2.50 mm0.0984″ | #40 |
| M3.5×0.6 | — | 3.50 mm0.1378″ | 2.90 mm0.1142″ | #33 |
| M4×0.7 | — | 4.00 mm0.1575″ | 3.30 mm0.1299″ | #30 |
| M5×0.8 | — | 5.00 mm0.1969″ | 4.20 mm0.1654″ | #19 |
| M6×1.0 | — | 6.00 mm0.2362″ | 5.00 mm0.1969″ | #9 |
| M7×1.0 | — | 7.00 mm0.2756″ | 6.00 mm0.2362″ | 6.0 mm |
| M8×1.25 | — | 8.00 mm0.315″ | 6.80 mm0.2677″ | H |
| M9×1.25 | — | 9.00 mm0.3543″ | 7.80 mm0.3071″ | 7.8 mm |
| M10×1.5 | — | 10.00 mm0.3937″ | 8.50 mm0.3346″ | 8.5 mm |
| M11×1.5 | — | 11.00 mm0.4331″ | 9.50 mm0.374″ | 9.5 mm |
| M12×1.75 | — | 12.00 mm0.4724″ | 10.20 mm0.4016″ | 10.2 mm |
| M14×2.0 | — | 14.00 mm0.5512″ | 12.00 mm0.4724″ | 12.0 mm |
| M16×2.0 | — | 16.00 mm0.6299″ | 14.00 mm0.5512″ | 14.0 mm |
| M18×2.5 | — | 18.00 mm0.7087″ | 15.50 mm0.6102″ | 39/64 |
| M20×2.5 | — | 20.00 mm0.7874″ | 17.50 mm0.689″ | 44/64 |
| M22×2.5 | — | 22.00 mm0.8661″ | 19.50 mm0.7677″ | 19.5 mm |
| M24×3.0 | — | 24.00 mm0.9449″ | 21.00 mm0.8268″ | 53/64 |
| M27×3.0 | — | 27.00 mm1.063″ | 24.00 mm0.9449″ | 24.0 mm |
| M30×3.5 | — | 30.00 mm1.1811″ | 26.50 mm1.0433″ | 1-3/64 |
| M33×3.5 | — | 33.00 mm1.2992″ | 29.50 mm1.1614″ | 29.5 mm |
| M36×4.0 | — | 36.00 mm1.4173″ | 32.00 mm1.2598″ | 32.0 mm |
| M39×4.0 | — | 39.00 mm1.5354″ | 35.00 mm1.378″ | 1-24/64 |
| M42×4.5 | — | 42.00 mm1.6535″ | 37.50 mm1.4764″ | 37.5 mm |
| M45×4.5 | — | 45.00 mm1.7717″ | 40.50 mm1.5945″ | 1-38/64 |
| M48×5.0 | — | 48.00 mm1.8898″ | 43.00 mm1.6929″ | 43.0 mm |
Quick answer: what is a tap drill size?
A tap drill is the hole you drill before running the tap — smaller than the finished thread, not the bolt clearance diameter. Too small overloads the tap; too large weakens thread engagement.
PREMSA's calculator covers metric coarse/fine, UNC, UNF, and NPT with cutting taps at 75% thread height and forming-tap formulas. Results show mm, inches, and the closest stocked drill.
Cutting taps use divisor 76.98; forming taps use 175. Same thread, different hole — always select tap type before quoting or programming CAM.
Common tap drills at 75% (cutting tap): 1/4-20 UNC → #7 (~0.201″ / 5.1 mm) | M6×1.0 → ~5.0 mm | M8×1.25 → ~6.8 mm | 10-32 UNF → #21 (~0.159″ / 4.04 mm)
Complete tap drill size guide
How tap drill sizing works
A tap cuts internal threads in a machined part. Before tapping, you drill a smaller hole — the tap drill. If the hole is too small, torque spikes and breakage risk goes up. If it is too large, threads are shallow and weak.
For cutting taps, this calculator uses standard 75% tap drill charts — the same shop reference tables machinists use daily. Forming taps use the roll-tap formula with divisor 175 instead of 76.98.
An incorrect tap drill can turn a straightforward threading operation into scrap. Validate the hole diameter before programming a CNC tapping cycle, releasing a drawing, or submitting a STEP file for quote.
Tap drill formulas (60° UNC, UNF, and metric)
For straight 60° threads, tap drill diameter depends on major diameter, pitch, and the thread height percentage (Hp) you want left in the part. These formulas follow Machinery's Handbook practice and match common shop charts.
Cutting tap · inch (UNC / UNF)
D = D_major − Hp / (76.98 × TPI)
Cutting tap · inch (pitch P)
D = D_major − (Hp × P) / 76.98
Cutting tap · metric
D = D_major − (Hp × P) / 76.98
Forming tap · inch (UNC / UNF)
D = D_major − Hp / (175 × TPI)
Forming tap · inch (pitch P)
D = D_major − (Hp × P) / 175
Forming tap · metric
D = D_major − (Hp × P) / 175
- D
- Tap drill diameter (pre-tap hole), in mm or inches.
- D_major
- Nominal major thread diameter (bolt/screw OD), same units as D.
- P
- Thread pitch: mm on metric threads, or P = 1 ÷ TPI on inch threads.
- TPI
- Threads per inch (UNC / UNF inch threads only).
- Hp
- Thread height as % of the full 60° profile; 75% is the usual shop value.
- 76.98
- Divisor for cutting taps (60° UN / ISO profile).
- 175
- Divisor for forming taps (roll tap).
NPT pipe threads are tapered — use pipe tap drill tables; the formulas above do not apply.
Cutting tap vs forming tap
Drilling for a cutting tap is not the same as drilling for a forming tap that displaces metal instead of removing it. Both methods target the same Hp (default 75%); only the divisor changes.
- Cutting tap — Removes chips; uses divisor 76.98 — smaller hole for the same Hp and thread strength target.
- Forming tap (roll tap) — Displaces metal without chips; uses divisor 175 — larger hole at the same Hp.
- NPT pipe threads — Tapered for sealing — tap drills come from pipe thread tables, not straight-thread formulas.
Shop tip: In blind holes, hard materials, or form taps, a slightly larger drill lowers torque and extends tap life. Always verify against your drawing, thread class, and the tap you will actually run.
Picking the right standard drill
Your calculated tap drill will almost never match a stocked size exactly. Round up to the next number, letter, fractional, or metric drill (see the reference tables below). Rounding up cuts engagement by 1–3% — that is the safe shop practice. Rounding down overloads the tap.
Thread systems in the calculator
UNC (coarse) and UNF (fine) cover most inch fasteners — e.g. #0-80 is UNF only, not UNC. Metric Coarse and Metric Fine are the most common ISO threads on CNC parts. NPT is for tapered pipe connections.
- Metric coarse / fine — ISO threads on most CNC machined parts — M3 through M24 in the tables below.
- UNC / UNF — Inch fasteners — 1/4-20, 10-32, and fractional sizes in the calculator and thread tables.
- NPT — Tapered pipe threads — select NPT in the calculator for pipe tap drill reference values.
Why tap drill diameter matters for CNC
Thread strength is not defined by nominal size alone. Thread percentage, engagement depth, part material, and manufacturing method all influence the final result. A difference of a few tenths of a millimeter can affect joint strength, tap life, cycle time, thread quality, and scrap rate.
Design engineers, CAM programmers, quality teams, and CNC operators rely on tap drill charts during part development. For DFM on threaded features, see PREMSA's CNC Design Guide.
Popular tap drill size searches
Quick answers to the tap drill lookups machinists and engineers search most often.
- What tap drill for 1/4-20?
- 1/4-20 UNC (coarse) → #7 drill ≈ 0.201″ (5.1 mm) at 75% thread with a cutting tap. Use the calculator above for forming taps or different thread heights.
- M6 tap drill size in mm
- M6×1.0 (metric coarse) → ~5.0–5.1 mm cutting tap at 75%. M6×0.75 (fine) → ~5.25 mm. Select Metric Coarse or Metric Fine in the calculator.
- M8 tap drill size
- M8×1.25 (coarse) → ~6.8 mm cutting tap at 75%. Fine M8×1.0 needs a slightly larger hole — use the calculator for exact mm and inch values.
- 10-32 tap drill size
- 10-32 UNF → ~#21 drill ≈ 0.159″ (4.04 mm) at 75% with a cutting tap. Search 10-32 in the calculator for the full result.
- Cutting tap vs forming tap drill size
- Cutting taps need a smaller hole (divisor 76.98). Forming taps need a larger hole (divisor 175). Same thread, different drill — select tap type in the calculator.
- What does 75% thread height mean?
- 75% is how full the thread profile is compared with a theoretical 100% thread — the standard shop default. Lower % = larger hole, easier tapping, slightly weaker threads.
- Metric tap drill chart
- Use Metric Coarse or Metric Fine in the calculator, or scroll to the Threads table below for M3 through M24 tap drill diameters in mm and inches.
- NPT tap drill chart
- NPT pipe threads are tapered — tap drills come from pipe thread tables, not straight-thread formulas. Select NPT in the calculator for reference sizes.
- Clearance hole vs tap drill
- Tap drill = pre-thread hole (smaller). Clearance hole = bolt passes through (larger). See Screw Fit — Inch/Metric tables below for close and free fit ranges.
- Why does my calculated size not match a drill in the catalog?
- The math returns an exact theoretical diameter; shops only stock standard drills. Round up to the next available size — the calculator shows both calculated and approximate stocked drill.
How to use this tap drill calculator
- PREMSA publishes this tap drill size calculator for metric coarse/fine, UNC, UNF, and NPT threads — with 75% thread height cutting-tap charts, forming-tap formulas, and closest standard drill recommendations in mm and inches.
- A tap drill is the hole drilled before tapping. It must be smaller than the finished thread — not the bolt clearance diameter. 1/4-20 UNC → #7 drill (~0.201″ / 5.1 mm). M6×1.0 → ~5.0 mm cutting tap at 75%.
- Cutting taps need a smaller hole than forming taps (roll taps) for the same thread. The calculator applies divisor 76.98 vs 175 automatically — do not swap tap types without recalculating.
- Calculated diameters are theoretical; shops stock number, letter, fractional, and metric drills. Round up to the next available size — see the Drill Bit Size Chart for full catalog diameters.
- For production CNC drilling and tapping at PREMSA in Monterrey, call out thread standard, class, depth, and tap type on your drawing — then request a quote with STEP and drawing.
Related Resources
- Chart
Tap & Drill Size Chart
UNC, UNF, and metric tap drill table with clearance drills at 75% thread.
View chart - Chart
Drill Bit Size Chart
Number, letter, and fractional drill diameters in mm and inches—full standard drill catalog.
View chart - Chart
ISO 2768 Tolerance Chart
ISO 2768-1 linear and angular general tolerances with lookup tool.
View chart - Chart
ISO 286 Fit & Tolerances Chart
IT grades and preferred hole-basis / shaft-basis fits for mating bores and shafts.
View chart - Tool
Fit & Clearance Calculator
Instant hole/shaft limit sizes and assembly clearance for H7/g6, H7/h6, and other ISO 286 pairs.
Open tool - Guide
CNC Design Guide for Machining
DFM rules for holes, threads, tolerances, and manufacturability on CNC parts.
Read guide
Drill & tap questions
- What is a tap drill size?
- It is the hole diameter you drill before running the tap. Too small and the tap loads up, torque spikes, and breakage risk goes up. Too large and threads are weak. The calculator above returns that size in millimeters and inches, plus the closest standard drill bit you would typically grab in a shop.
- What tap drill do I use for 1/4-20?
- 1/4-20 means a 1/4 inch screw with 20 threads per inch (UNC coarse). With a cutting tap at the usual 75% thread height, the ideal hole is about 5.1 mm (0.201″). In practice you almost always drill with a #7 bit — the nearest standard size in stock, not an odd fraction. A slightly larger hole makes tapping easier in hard material, but the thread holds a little less.
- What tap drill do I use for M6?
- M6×1.0 is a 6 mm metric screw with 1 mm pitch (coarse). With a cutting tap at 75%, the tap drill is about 5.0–5.1 mm. Fine-pitch M6×0.75 needs a slightly larger hole (~5.25 mm). Pick Metric Coarse or Metric Fine in the calculator to see both mm and inch equivalents.
- What is the difference between a cutting tap and a forming tap?
- A cutting tap removes chips and needs a smaller hole. A forming tap (roll tap) displaces metal without chips and needs a larger hole for the same thread strength target. Select the tap type in the calculator — the drill size is not interchangeable between the two.
- What does 75% thread height mean?
- It is not how deep the hole is in the part — it is how full the thread profile is compared with a theoretical 100% thread. 75% is the most common shop default: strong enough for most joints without overloading the tap. A lower percentage means a larger hole, easier tapping, and slightly weaker threads.
- What are UNC, UNF, metric, and NPT threads?
- UNC and UNF are inch threads (coarse and fine). Metric coarse and metric fine are the ISO threads most common on CNC parts. NPT is a tapered pipe thread — different rules apply; select NPT in the calculator for pipe tap drill reference values.
- Why does my calculated size not match a drill in the catalog?
- The math returns an exact theoretical diameter; shops only stock standard drills (number, letter, fractional, or metric). The correct approach is to round up to the next available size. The calculator shows both the calculated diameter and the approximate stocked drill you would use in production.
- Does the same tap drill work for blind and through holes?
- Usually yes — the same tap drill applies to through and blind holes. For deep blind holes, hard alloys, or form taps, confirm with your shop: a slightly larger drill can reduce torque and help avoid breaking the tap at the bottom.
- Are NPT pipe threads drilled the same as metric?
- No. NPT threads are tapered for pipe sealing; tap drills come from pipe thread tables, not the straight-thread formula. Choose NPT in the calculator to look up those reference sizes.
- How do I validate tap drill size before sending parts to CNC?
- Check your drawing for thread standard (M6, 1/4-20, NPT, etc.), class, depth, and whether the process uses cutting or forming taps. Use this calculator when quoting and releasing drawings; the shop confirms with stocked drills and first-article inspection in production.
It is the hole diameter you drill before running the tap. Too small and the tap loads up, torque spikes, and breakage risk goes up. Too large and threads are weak. The calculator above returns that size in millimeters and inches, plus the closest standard drill bit you would typically grab in a shop.
1/4-20 means a 1/4 inch screw with 20 threads per inch (UNC coarse). With a cutting tap at the usual 75% thread height, the ideal hole is about 5.1 mm (0.201″). In practice you almost always drill with a #7 bit — the nearest standard size in stock, not an odd fraction. A slightly larger hole makes tapping easier in hard material, but the thread holds a little less.
M6×1.0 is a 6 mm metric screw with 1 mm pitch (coarse). With a cutting tap at 75%, the tap drill is about 5.0–5.1 mm. Fine-pitch M6×0.75 needs a slightly larger hole (~5.25 mm). Pick Metric Coarse or Metric Fine in the calculator to see both mm and inch equivalents.
A cutting tap removes chips and needs a smaller hole. A forming tap (roll tap) displaces metal without chips and needs a larger hole for the same thread strength target. Select the tap type in the calculator — the drill size is not interchangeable between the two.
It is not how deep the hole is in the part — it is how full the thread profile is compared with a theoretical 100% thread. 75% is the most common shop default: strong enough for most joints without overloading the tap. A lower percentage means a larger hole, easier tapping, and slightly weaker threads.
UNC and UNF are inch threads (coarse and fine). Metric coarse and metric fine are the ISO threads most common on CNC parts. NPT is a tapered pipe thread — different rules apply; select NPT in the calculator for pipe tap drill reference values.
The math returns an exact theoretical diameter; shops only stock standard drills (number, letter, fractional, or metric). The correct approach is to round up to the next available size. The calculator shows both the calculated diameter and the approximate stocked drill you would use in production.
Usually yes — the same tap drill applies to through and blind holes. For deep blind holes, hard alloys, or form taps, confirm with your shop: a slightly larger drill can reduce torque and help avoid breaking the tap at the bottom.
No. NPT threads are tapered for pipe sealing; tap drills come from pipe thread tables, not the straight-thread formula. Choose NPT in the calculator to look up those reference sizes.
Check your drawing for thread standard (M6, 1/4-20, NPT, etc.), class, depth, and whether the process uses cutting or forming taps. Use this calculator when quoting and releasing drawings; the shop confirms with stocked drills and first-article inspection in production.
Ready for your next project with PREMSA?
Upload your STEP file, set material and quantity, and get DFM review with clear lead times and an online quote.