Why Drilled Holes Go Oversize, Taper, or Burr

By Bradley Taylor · August 2026

A twist drill is a roughing tool. On a good day it makes a hole close to size with a decent finish, and on a bad day it makes something oval, tapered, and furry at both ends. Each of those failures has its own cause, and once you can read the symptoms, the fix is usually obvious. Here is how I sort them out at the machine.

When the hole runs big, look at the grind first

The classic drilled hole oversize cause is a drill with unequal lips. A drill has two cutting lips, and for the tool to cut on center they need to be the same length and ground at the same angle. When one lip is longer or steeper than the other, one lip does most of the cutting and the point ends up off the centerline of the shank. The drill then swings around that offset point as it spins, sweeping a circle bigger than its own diameter. The hole runs oversize by roughly the amount of the mismatch, and it will do it every time, in every material, because the error is ground into the tool.

This is almost always a hand regrind. A drill fresh off a quality grinder is close to symmetric. A drill touched up freehand on the pedestal grinder by someone in a hurry is a coin flip. If a drill that used to make good holes suddenly cuts big after a trip to the grinder, you already have your answer. Check it with a drill point gauge, or just drill a test hole in scrap and mic it before the drill touches the real part. A drill that measures 0.375 and makes a 0.381 hole is telling you about six thousandths of lip mismatch, approximately, and no amount of feed and speed adjustment will fix a grind.

The chisel edge matters too. A worn or badly ground chisel edge does not center itself well, so the drill skates for a moment before it bites. That wandering start gets recorded in the top of the hole and can leave the whole hole big and ugly even after the drill settles down.

Other ways a hole grows

If the grind checks out, look at everything holding the drill. Runout in the chuck or holder does the same thing as unequal lips, because the drill is again spinning about an axis that is not its own centerline. A drill held with 0.003 of runout will cut a hole roughly that much oversize near the top. Chase it with an indicator on the drill body, and clean the chuck jaws and the taper while you are in there. A bent drill is the same failure in a cheaper package. Roll it on a flat surface and watch the point.

Walking at the start is the last of the usual suspects. A drill entering bare material on a surface that is not flat, or entering at the edge of a previous feature, will slide sideways before it establishes a hole. A spot drill fixes that, but only if the spot angle is right. The spot should be the same angle as the drill point or larger, so the drill lips touch down before the outer corners do. Spot a 135 degree drill with a 90 degree spot and the corners land first, chatter, and chip, and the hole starts wrong anyway.

Taper and bellmouth

A hole that is big at the top and correct at the bottom usually got bellmouthed at entry. The unsupported drill flexes when it first contacts the part, wanders a little, and then straightens out once the margins engage the hole wall and start guiding it. The cure is rigidity. Shorten the stickout, use a stub length drill for the first portion of a deep hole, and spot properly so the drill has something to follow. A hole that tapers steadily along its length points instead at worn margins. The margins are what size the hole behind the point, and once they wear the drill cuts progressively smaller as it goes down. General lack of rigidity in the setup, a loose quill, or a part that moves under thrust will produce the same family of shapes, so check the whole stack, not just the tool.

Out of round and lobed holes

Thin parts and poorly supported parts make lobed holes. The material flexes away from the cutting lips, springs back, and gets cut again, and the result is a hole that mics fine in one direction and undersize in another, sometimes distinctly three lobed. Sheet metal on soft parallels is the textbook case. Support the part directly under the hole, clamp close to the cut, and the lobing mostly goes away. The drill was never the problem there.

Burrs at entry and exit

An entry burr comes from a dull drill pushed too hard. Sharp lips shear the surface cleanly, while dull ones plow material up and out around the rim. Sharpen the drill and back off the feed and the entry cleans up. Exit burrs are a different mechanism. As the point breaks through, the thin remaining web of material stops being cut and starts being pushed, and the drill shoves that last bit out the bottom as a burr instead of shearing it. The fixes follow from the cause. Keep the drill sharp, drop the feed just before breakthrough, and back up the exit with sacrificial material so the web stays supported until it is cut. In sheet, a higher point angle helps because the flatter point breaks through more evenly and leaves a smaller exit burr.

Finish problems

A torn, smeared hole wall in gummy material at low speed is usually built up edge. Material welds to the lips, grows, and breaks off into the finish. More speed and better coolant usually cure it. Rings or witness marks partway down a deep hole are pecking scars, left each time the drill re-enters and re-establishes the cut. And in deep holes generally, if coolant cannot reach the point, finish and size both fall apart, because the drill is cutting hot and packing chips. Peck enough to clear, or use coolant fed drills when the depth justifies them.

When the answer is drill and ream

Some holes should never be finished with a drill at all. When the print wants real size and real finish, drill undersize, leave the right amount of stock, and let a reamer do the last operation. A reamer follows the existing hole and cleans up size and finish beautifully, but only if the drill left it something reasonable to work with. The drill size chart covers the standard sizes for picking that pre ream drill.

The short version is worth repeating. A drill is a roughing tool that sometimes behaves, and when it misbehaves, the shape of the bad hole tells you why. Big means grind or runout, bellmouth means flex at entry, taper means worn margins, and burrs mean dull edges and pushed material. Start from the symptom and work backward. For starting speeds and feeds by material, the speeds and feeds calculator has a drilling mode that will get you close.

As always, this is general practice, not a spec. Prints, customer requirements, and the governing standard win every argument.