Drills: sizes, point angles and reaming

November 3, 2026  ·  Indumor

On a 10 mm drill the chisel edge is about 2 mm wide: a fifth of the diameter that crushes the material instead of cutting it, and that accounts for a third to a half of the thrust. That is why a large drill wants a pilot hole or a split point, and why a badly ground drill, with one lip longer than the other, leaves holes that are oval and bigger than the drill. This chapter covers choosing the drill, grinding it and knowing what hole it will leave. Tap drills are in chapters 4 to 6 and speeds in chapter 9.

Drill anatomy and point angles

A twist drill cuts with two lips that meet at the chisel edge; behind each lip the flank falls away at a clearance angle so the heel does not rub, and along the body two narrow lands, the margins, ride the wall and set the diameter. The point angle of a general-purpose drill is 118°; the helix of the type N drill is about 30°. DIN 1836 defines three helix types (N for steel and cast iron, H slow for brass and hard or brittle materials, W fast for aluminum and soft materials) and DIN 1412 five point forms.

When grinding by hand three things matter: that both lips are the same length and make the same angle with the axis, that there is clearance (8° to 12°; you can see it because the lip is the highest part of the flank) and that the chisel edge is not left long. A lip longer than the other does all the work, the drill walks, the hole comes out oversize and the drill breaks sooner. Check it with a drill point gauge or by measuring both lips with a caliper.

Standard series: DIN 338, 340, 345 and Morse tapers

The everyday drill is the DIN 338 jobber, straight shank up to 20 mm, diameter toleranced h8 (a 10 mm drill measures between 9.978 and 10.000). DIN 340 is the long series; DIN 1897 the stub, stiffer, for hand drills and machining centers. From 3 to 100 mm the DIN 345 has a Morse taper shank that goes straight into the lathe tailstock or the drill press spindle (taper dimensions are in chapter 11); the taper number depends on the diameter. Solid carbide drills (DIN 6537) belong on rigid machines with through-coolant and run three or four times the speed of HSS. In inch shops the equivalents are the jobber, taper-length and screw-machine series of ASME B94.11M.

Blind holes: the point takes depth

The cone of the point takes up depth, 0.3 times the diameter at 118°. If the drawing asks for a 20 mm deep blind hole at full diameter with a 12 mm drill, the depth stop goes at 20 + 3.6 = 23.6 mm, and there has to be wall beyond it. In a blind tapped hole you also add the chamfer of the tap, which does not thread to full diameter. The formula works for any point angle.

Clearance holes for bolts (ISO 273)

A bolt passes through a hole larger than its thread. ISO 273 gives three series: fine, for machined parts with accurate positions; medium, the usual one; coarse, for structures, folded sheet and parts where the holes have to absorb position errors. For an M10 that is 10.5, 11 or 12 mm. ASME B18.2.8 does the same job for inch screws.

Countersinks and counterbores

A flat countersunk screw (DIN 7991, ISO 10642) needs a 90° cone whose diameter at the surface is slightly larger than the theoretical head, so the head sits flush; ISO 15065 fixes countersinks only for ISO 7721 heads, up to M10, and the table gives a shop diameter and the depth that follows from the geometry. A socket head cap screw (DIN 912, ISO 4762) goes in a cylindrical counterbore per DIN 974-1, with a diameter that clears the key and a depth that hides the head. A 90° countersink also deburrs any hole, and two turns by hand are enough. Inch countersunk screws use an 82° head, not 90°, so the countersink has to match.

The DIN 7991 head is somewhat smaller (k = 1.7 mm on M3, 4.4 on M8 and 8.5 on M20): with these sizes it sits below the surface by 0.3 mm (M3) to 1.8 mm (M20).

DIN 974-1 fixes the diameter d2; the depth t is a guide value: the head height k plus a clearance.

Reaming: stock allowance and H7 reamers

A drill leaves a hole slightly larger than itself, 0.05 to 0.15 mm, and out of round; when the drawing calls for H7 (a bushing, a dowel pin, the seat of a small bearing) you drill undersize and finish with a reamer. The allowance must be small, 0.2 mm up to 10 mm diameter and 0.3 to 0.5 on large ones. Too little and the reamer rubs and dulls; too much and it loads up and cuts oversize. Run it at half the drill's rpm and two or three times the feed, with oil, and never back it out in reverse, because that scores the wall. H7 tolerances are in chapter 3.

Number and letter drills

American drawings and manuals name small drills by a number (from #80, 0.0135 in, to #1, 0.228 in) and medium ones by a letter (from A, 0.234 in, to Z, 0.413 in). The series is based on the 19th-century Stubs steel wire gauge and follows no formula; #7 is the tap drill for 1/4-20 and F for 5/16-18 (chapter 5). The sizes are those of ASME B94.11M, exact; the finder at the end converts a number or letter to millimeters and finds the closest one to a metric size.

Frequently asked questions

What size drill for an M8 clearance hole?

9 mm in the ISO 273 medium series, which is the usual one. The fine series calls for 8.4 mm (machined parts with accurate positions) and the coarse series 10 mm (structures and folded sheet). For M10: 10.5, 11 or 12 mm.

What point angle does a drill for steel have?

118°, with 8° to 12° of lip clearance, for structural and low-carbon steel. For quenched-and-tempered and stainless steels, 130° to 135° with a split point, which centers itself and needs less thrust. Aluminum takes a fast helix (type W); brass a slow one (type H).

How many millimeters is a #7 drill?

0.201 in, which is 5.105 mm; it is the tap drill for 1/4-20 UNC. Letter drills follow #1 (0.228 in): A is 0.234 in (5.944 mm) and Z is 0.413 in (10.490 mm).

Sources: ASME B94.11M-1993, Twist Drills, Straight Shank and Taper Shank; DIN 338, DIN 340, DIN 345, DIN 1897, DIN 1869, DIN 6537 (twist drill series); DIN 1836 (helix types N, H and W); DIN 1412 (point forms); ISO 273:1979 (clearance holes); ISO 10642 and DIN 7991 (countersunk head screws); ISO 15065 (countersinks for ISO 7721 heads); DIN 974-1 (counterbores); DIN 912 / ISO 4762; ISO 286-2 (H7 tolerance); Machinery's Handbook, 31st edition (2020).