ISO metric thread chart: pitch, tap drill and clearance holes
Published September 25, 2026 — from M1.6 to M36: coarse and fine pitch, tap drill, ISO 273 clearance holes and wrench sizes, in one filterable table. Plus the formula to remember and the SOLIDWORKS settings that prevent mistakes.
The chart: ISO coarse pitch, M1.6 to M36
All values are in millimetres. The tap drill is the standard shop value (D − P rounded to a stock drill). Clearance holes follow ISO 273: the medium series is the default. Wrench sizes are ISO across-flats (ISO 4032 nut / ISO 4017 hex bolt) and the hex key for ISO 4762 socket head cap screws.
Remember without a chart: M6 → 5, M8 → 6.8, M10 → 8.5, M12 → 10.2. These four sizes cover most general engineering work.
1. Fine pitch: the sizes you actually meet
Fine pitch is used when you need better resistance to loosening (vibration), fine adjustment, or a thin wall that can't take a deep thread. It is always written with the pitch: M12 × 1.5. With no pitch stated, it's coarse.
Clearance holes and wrench sizes are the same as for coarse pitch: only the tap drill changes.
2. The D − P formula, and when to deviate
Drill diameter = nominal diameter − pitch. It's the only formula you need: it gives about 75% thread height, which keeps nearly all the strength while limiting the load on the tap (and so breakage).
- Form tapping (roll tap, chipless): the hole is larger, about D − 0.5 × P. M6 → 5.5 mm. Using D − P breaks the tap.
- Hard materials or stainless: going up a tenth (M8 → 6.9) relieves the tap, at the cost of slightly shallower thread.
- Thread inserts (Helicoil type): they have their own drills, larger than the nominal size. Never apply this chart.
3. Choosing the clearance hole: fine, medium or coarse
The clearance hole is not a matter of taste: it's a matter of position tolerance. Two parts joined by four screws only assemble if the hole clearance absorbs spacing errors on both sides.
- Fine series: precise positioning, both parts CNC-machined. Little margin at assembly.
- Medium series: the default for general engineering. If in doubt, use this one.
- Coarse series: sheet metal, welded frames, raw parts, on-site fitting. Add a washer.
4. Depths: thread engagement and blind holes
Thread engagement depends on the tapped part's material: 1 × d in steel, 1.5 × d in cast iron, 2 × d in aluminium. Beyond that you gain almost nothing: the first three or four threads carry most of the load.
In a blind hole, drill deeper than the thread: a machine tap has a 2 to 5 incomplete-thread chamfer, and chips need room. Allow at least thread length + 3 pitches, and dimension both depths separately on the drawing.
Once the thread is sized, it still has to be tightened to the right torque: the 8.8, 10.9 and 12.9 tightening torque chart gives values from M3 to M36, with a calculator by friction.
5. In SOLIDWORKS: let the Hole Wizard do the work
The Hole Wizard already knows all these values (ISO standard, Tapped hole or Clearance type, Close / Normal / Loose fit). Using it instead of a plain circular cut changes three things:
- The drawing dimensions itself: the hole callout (M8 - 6H, depth…) is generated and stays correct if the hole changes.
- Hole tables on drawings fill in automatically, size and type included.
- Consistency between parts: Hole Alignment and the Hole Series feature check that clearance and tapped holes match across parts.
The classic trap is holes "drawn by hand" with a typed-in diameter: it's one of the most common SOLIDWORKS mistakes I see in audits, and it always ends with a wrong drawing in the shop. If your teams share a fastener library, its codification and properties matter just as much — see SOLIDWORKS codification and properties.
6. FAQ
What drill size for an M8 tap?
6.8 mm. M8 has a 1.25 mm coarse pitch, and the drill diameter is D − P: 8 − 1.25 = 6.75, rounded to the standard 6.8 mm drill. For M8 × 1 (fine pitch), drill 7 mm.
How do I calculate the tap drill size?
Nominal diameter minus pitch: D − P. M6 (pitch 1) → 5 mm; M10 (pitch 1.5) → 8.5 mm; M12 (pitch 1.75) → 10.25, rounded to 10.2 mm. The formula gives roughly 75% thread depth, the right trade-off between strength and tapping torque.
What clearance hole for an M6 screw?
6.6 mm in the medium series (ISO 273), the default choice. 6.4 mm in the fine series when positioning matters, 7 mm in the coarse series when hole-spacing tolerances are loose.
What is the minimum thread engagement?
Shop rule: 1 × d in steel, 1.5 × d in cast iron, 2 × d in aluminium and soft alloys. Beyond that the strength gain is negligible: the first threads carry the load.
Why a 16 mm wrench and not 17 for M10?
Because ISO reduced some across-flats sizes: M10 → 16 (formerly DIN 17), M12 → 18 (formerly DIN 19), M14 → 21 (formerly DIN 22), M22 → 34 (formerly DIN 32). Both still coexist in workshops: check the standard of the fasteners you order.