Drilling RPM calculator

Drilling: the tool that cuts at zero speed in the middle

A drill is stranger than it looks. The outer corners travel at full cutting speed, but the centre of the drill travels at zero — the very middle of the point cannot cut at all, it simply extrudes material sideways under enormous pressure. That dead zone is called the web, and it explains most of what goes wrong when drilling. It is why a large drill needs so much thrust, why it wanders when starting on a curved or uneven surface, and why the calculated speed here refers to the outside diameter: it is the only part of the tool actually doing proper cutting.

Why the pilot hole is not optional above a certain size

Because the web does not cut, a large drill spends much of its effort pushing material out of the way. A pilot hole removes exactly that problem: drill first with a diameter roughly equal to the web thickness — for most standard drills that is around 15 to 20% of the final diameter — and the big drill suddenly needs far less thrust, wanders less and produces a rounder hole. Do not go the other way and drill a pilot that is too large, though: if the pilot is wider than the drill point can span, the outer corners bite in without support and the drill will grab, especially in brass and other free-cutting materials.

Chip evacuation, and why depth changes everything

In milling the chip falls away. In drilling it has to travel back up the flutes past the tool, through a hole full of heat, and everything about a deep hole makes that harder. Up to about three diameters deep you can usually drill straight through. Beyond that, chips start to pack, and packed chips are the direct cause of most broken drills: the flutes fill, the chip can no longer escape, pressure rises and the tool seizes. Peck drilling — retracting periodically to clear — is the standard answer, and beyond roughly five diameters it becomes essential rather than cautious. Reduce your feed as depth increases and watch what comes out: long continuous spirals mean things are going well, while dust or short broken fragments mean the edge is dull or rubbing.

Why stainless steel runs so much slower than mild steel

Stainless is not simply harder — it work-hardens. Deform its surface without cutting cleanly through it and the material directly under the tool becomes considerably harder than it was a moment ago. That produces a vicious circle in drilling: a dull edge or a hesitant feed rubs instead of cutting, the surface hardens, the hardened layer resists the edge even more, and within seconds the drill is polishing a glazed spot it can no longer enter. Stainless therefore wants a lower cutting speed but a firm, positive feed — the mistake most people make is easing off when it gets difficult, which is exactly the wrong response. Get through the skin and keep going.

Breakout, and the moment the hole is nearly finished

The last fraction of a millimetre before the drill exits is when things go wrong. The material ahead of the point is now a thin unsupported membrane, the drill wants to pull itself through it, and on a drill press that shows up as a grab, a snatched workpiece, or a torn ragged exit. Ease the feed as you approach breakthrough, and if the exit face matters, clamp a sacrificial backing piece behind the work so the drill exits into that instead of into air. On thin sheet the problem is worse still, because the drill point can punch through before the outer corners have finished the hole, leaving a triangular tear — that is what step drills and sheet-metal-specific points exist for.

Reading the chips, and when the calculated number is wrong

These figures assume a sharp standard drill, reasonable clamping and some cooling. The chips will tell you within seconds whether that assumption holds. Two smooth continuous spirals coming out steadily means speed and feed are in balance. Blue or brown chips mean too much heat, usually from too high a speed. Dust or powder means the edge is rubbing, not cutting, and something is dull. A squealing noise is the same message, more urgently. And be honest about the drill itself: a resharpened bit with unequal lip lengths cuts oversize with one lip doing all the work, and no calculator can compensate for that.

How drill speed is calculated

Every material has a preferred cutting speed (Vc, in metres per minute) — how fast the drill's cutting edge should travel through it. The spindle speed follows from the drill diameter: n = (Vc × 1000) / (π × Ø). That's why a 3 mm drill spins much faster than a 20 mm drill in the same material: the small drill's edge covers far less distance per revolution.