Drill Point Depth Calculator

A twist drill does not cut a flat bottomed hole. Its two lips meet at an angle - 118 degrees for the standard general purpose grind - and they leave behind a conical impression whose depth is fixed by that angle and the diameter.

The geometry is a single right triangle. The outer corner of the lip is half a diameter from the axis, and the tip sits below it by that half diameter divided by the tangent of half the included angle. At 118 degrees that comes out at 0.30043 times the diameter, which is why the shop rule of "about three tenths of the diameter" is so reliable - it is very nearly exact.

Everything else on this page is a consequence. The machine controls where the tip goes; the useful hole starts a point length above it. Whether that matters depends on which end of the hole you care about.

Ask for a hole an inch deep, programme an inch, and you get 0.85 inches of full diameter from a half inch drill. The remaining 0.15 is a cone that narrows to nothing.

For most clearance holes nobody notices. For a tapped hole it matters a great deal, because the shortfall lands exactly where the deepest threads would have been - and those are the threads someone specified a depth for in the first place. A tap run into a hole that is short simply bottoms, and either the tap breaks or the operator backs off and the thread is shallower than the drawing asks.

The habit worth forming is to work backwards. Decide the full thread depth needed, add a couple of pitches for the tap's chamfer to run out into, and that is the full diameter depth. Then add the point length, and that is the number to programme.

The mistake here is more consequential than the blind hole one, because it damages tools rather than just parts.

To break through an inch of plate with an inch drill, the tip has to travel 1.300 inches before the outer corners of the lips reach the far face - and then a little more before they finish cutting. Programme the material thickness and the drill is still buried when the programme says it is finished. What happens next is that the remaining thin ring of metal is torn out rather than cut, usually with a bang, a poor exit burr, and a shock load on a tool that is at its most vulnerable.

The breakout moment is genuinely the worst part of a drilling cycle. The material ahead of the point has thinned to nothing and lost its support, so it deflects instead of shearing, and the drill can grab and pull itself into the work. On a drill press with a loose quill this is how bits snap. A generous clearance past the calculated depth is cheap insurance, and slowing the feed for the last part of the cut is cheaper still.

The 118 degree standard is a compromise that has been around long enough to look like a law of nature. It is not.

A 135 degree point is shallower, so it wastes less depth, and it is usually supplied as a split point - the web is thinned and relieved so the drill starts on its own rather than skating. That self centring is generally the reason to choose it, and it removes the need for a separate spot drill on a lot of work. It also spreads cutting over a longer lip, which helps in tough and work hardening materials. The cost is thrust: a shallower point pushes harder for the same feed, so it wants a machine that can hold the work still.

Shallower angles still - 90 and 60 degrees - are for spotting and chamfering rather than depth. And there is a subtlety about combining them worth knowing: a spot drill should have a *wider* included angle than the drill that follows it, so the drill's outer corners contact first and centre it. A spot narrower than the drill lets the drill tip land inside the cone with its corners free, which is exactly the wandering the spot was supposed to prevent.