- Home
- Technical data
Tap Drill Sizes for Metric Coarse Threads: M1.6 to M24 Chart
To tap an ISO metric coarse thread with a cutting tap, drill a hole the size of the thread minus the pitch. The common sizes: M3 → Ø2.5, M4 → Ø3.3, M5 → Ø4.2, M6 → Ø5.0, M8 → Ø6.8, M10 → Ø8.5, M12 → Ø10.2.
Tap drill chart, M1.6 to M24
All sizes in millimetres, for ISO metric coarse threads (ISO 261) cut with a standard cutting tap. The minor diameter columns are the limits of the finished internal thread for the usual 6H tolerance class (ISO 965-1); a correct tap drill lands between them. "Try it" opens a plate with four tapping-size holes in the generator.
| Thread | Pitch | Tap drill | Minor Ø min | Minor Ø max (6H) | Try it |
|---|---|---|---|---|---|
| M1.6 | 0.35 | 1.25 | 1.221 | 1.321 | Make a plate |
| M2 | 0.4 | 1.6 | 1.567 | 1.679 | Make a plate |
| M2.5 | 0.45 | 2.05 | 2.013 | 2.138 | Make a plate |
| M3 | 0.5 | 2.5 | 2.459 | 2.599 | Make a plate |
| M3.5 | 0.6 | 2.9 | 2.850 | 3.010 | Make a plate |
| M4 | 0.7 | 3.3 | 3.242 | 3.422 | Make a plate |
| M5 | 0.8 | 4.2 | 4.134 | 4.334 | Make a plate |
| M6 | 1 | 5 | 4.917 | 5.153 | Make a plate |
| M8 | 1.25 | 6.8 | 6.647 | 6.912 | Make a plate |
| M10 | 1.5 | 8.5 | 8.376 | 8.676 | Make a plate |
| M12 | 1.75 | 10.2 | 10.106 | 10.441 | Make a plate |
| M14 | 2 | 12 | 11.835 | 12.210 | Make a plate |
| M16 | 2 | 14 | 13.835 | 14.210 | Make a plate |
| M18 | 2.5 | 15.5 | 15.294 | 15.744 | Make a plate |
| M20 | 2.5 | 17.5 | 17.294 | 17.744 | Make a plate |
| M22 | 2.5 | 19.5 | 19.294 | 19.744 | Make a plate |
| M24 | 3 | 21 | 20.752 | 21.252 | Make a plate |
Tap drill sizes are D − P, rounded where needed to a common drill size (M8 → 6.8, M12 → 10.2). Some charts round M2.5 to 2.1 mm; any drill inside the minor diameter limits works.
Why the drill is D − P
A tap does not cut the whole hole: it only cuts the thread form into the wall. The hole you drill becomes the thread's minor diameter, the inner tips of the internal thread. For an ISO metric thread, the smallest allowed minor diameter is D − 1.0825 × P (ISO 724), and the 6H tolerance lets it be a little larger.
D − P sits just above that minimum, so the thread has nearly full depth while leaving the tap a little room. A smaller drill makes tapping hard and breaks small taps; a larger drill gives shallower threads that strip more easily. The extra depth of a tighter hole adds little strength, which is why the standard sizes are not smaller.
Tapping tips
- Blind holes: drill deeper than the thread you need. A tap has a tapered lead at its tip that does not cut full threads, so allow a few extra pitches below the last full thread, plus room for chips.
- Thread length: as a rule of thumb, aim for at least 1 × D of full thread in steel and more (around 1.5 to 2 × D) in aluminium, cast iron and plastics. For loaded joints, check with the fastener supplier.
- Cutting fluid: use a tapping fluid on steel and aluminium, and back the tap off every turn or so to break the chip (not needed with spiral-flute or spiral-point taps).
- Forming taps: thread-forming (roll) taps need a larger hole than this chart gives. Use the tap maker's drill size.
- Countersink the hole lightly before tapping. It helps start the tap straight and stops the first thread lifting a burr.
- 3D printed parts: small FDM holes print undersize, so a printed tapping hole is often tight. Print the hole at the tap drill size and drill it out, or use heat-set threaded inserts, which last better in plastic.
Tapping holes vs clearance holes
The two are easy to mix up. The tapping hole is in the part that gets the thread and is smaller than the screw (Ø4.2 for M5). The clearance hole is in the part the screw passes through and is larger than the screw (Ø5.5 for M5, medium series). See the metric clearance hole sizes chart for those.
Tapping holes in Mechform
When you type a screw size like "4 M5 holes", Mechform draws clearance holes. For a part you will tap, give the drill size instead, for example "plate 80x50x8 with 4 holes, 4.2mm holes", or set Hole Ø in the Adjust panel. The drawing will show a plain Ø4.2 hole, so add the thread callout (for example "M5 × 0.8 - 6H, 4 holes") when you send it for manufacture.
Generate it now: plate with M5 tapping holes · block with M8 tapping holes
FAQ
What size drill for an M3 tap?
Use a 2.5 mm drill for an M3 × 0.5 coarse thread with a cutting tap. The 6H minor diameter of the tapped hole is 2.459 to 2.599 mm, so a 2.5 mm hole sits inside it.
What size drill for M4, M5 and M6 taps?
For metric coarse threads with a cutting tap: M4 × 0.7 → 3.3 mm, M5 × 0.8 → 4.2 mm, M6 × 1 → 5.0 mm.
What size drill for M8, M10 and M12 taps?
For metric coarse threads with a cutting tap: M8 × 1.25 → 6.8 mm, M10 × 1.5 → 8.5 mm, M12 × 1.75 → 10.2 mm.
How do I work out a metric tap drill size?
Subtract the pitch from the nominal diameter: tap drill = D − P. For M10 × 1.5 that is 10 − 1.5 = 8.5 mm. Round to the nearest standard drill that stays inside the minor diameter limits shown in the chart.
Does the same rule work for fine threads?
Yes, D − P works for ISO metric fine threads too, using the fine pitch. For example M10 × 1.25 → 8.75 mm, usually drilled 8.8 mm, and M12 × 1.5 → 10.5 mm.
Do thread-forming (roll) taps use the same drill size?
No. Forming taps push the material into shape instead of cutting it, so they need a larger hole than a cutting tap. Use the drill size given by the tap manufacturer.
Sources
- ISO 261:1998, ISO general purpose metric screw threads: general plan (coarse pitches)
- ISO 724:1993, ISO general-purpose metric screw threads: basic dimensions (D1 = D − 1.0825P)
- ISO 965-1:2013, ISO general purpose metric screw threads: tolerances, minor diameter tolerance TD1 grade 6
- ISO 2306:1972, Drills for use prior to tapping screw threads
Check critical dimensions against the current standard before manufacture.