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

Before blaming anything, know the baseline. A perfectly ground twist drill cuts oversize on purpose and by nature. Published figures put normal oversize for common sizes at roughly 0.002 to 0.005 inch, with maxima around 0.008 to 0.010 still inside the expected range. So the number that matters is never the absolute oversize. It is the change against what a known good drill of the same size and geometry makes in the same material and setup. Establish that baseline in scrap, and treat the difference as your problem to diagnose.

With the baseline in hand, the classic cause of a hole running genuinely big is a drill with unequal lips, and it pays to know there are two distinct versions of that. When the lips are equal angles but unequal lengths, the point sits off the centerline of the shank, and the hole comes out big by about twice the offset. When the lips are equal lengths but unequal angles, one lip does all the cutting, the unbalanced cutting force pushes the drill sideways, and the failure shows up as wander, bell shapes, and holes that are not straight rather than simply round and big. A rigid, bushed, or piloted setup shrinks both effects, which is why the same bad grind misbehaves worse hanging out of a drill chuck than it does in a screw machine.

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, and know what the gauge is telling you: the height difference you see on the gauge produces roughly twice that much oversize in the hole. Or skip the arithmetic, drill a test hole in scrap, and compare against your baseline. A 0.375 drill making a 0.381 hole is only a few thousandths over the published normal range, so compare before you condemn it. If a known good drill makes 0.377 in that setup and this one makes 0.381, the grind owns the difference, 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 is usually corner wear accumulating as the hole goes down. The outer corners of the lips are what scribe the diameter, and in abrasive material on a deep hole they can lose measurable size within a single hole. Two other causes look identical. The drill deflects at entry and then straightens once the margins are guided in the hole, and the drill's own ground in back taper starts to show once you are deep enough past an oversize entry. The margins behind the corners burnish and guide, they do not cut diameter, so margin wear alone will not taper a hole. 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

Lobed holes come in two flavors, and telling them apart is the whole diagnostic. An oval hole, two lobes, mics big in one direction and small ninety degrees away, and any micrometer will catch it. A three or five lobed hole is sneakier. An odd lobed shape reads nearly constant on any two point instrument, so it mics right at size while still rejecting a plug gauge. If a hole gauges bad but mics good, suspect odd lobing before you suspect the gauge. Three and five lobed holes are a documented habit of the two flute drill itself, a whirling vibration the drill falls into, and unequal lips make it worse. Thin and poorly supported parts add their own version, where the material flexes away from the lips, springs back, and gets cut again. Sheet metal on soft parallels is the textbook case. Support the part directly under the hole, clamp close to the cut, and that part of the lobing goes away.

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 cap 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 breakthrough cap 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.

Guided drilling, the fix nobody mentions

Almost every failure on this page shrinks when the drill is guided instead of hanging free. Drill bushings, a pilot hole drilled short and stubby before the full depth drill follows it, and short stub carbide drills all take flexibility out of the system, and flexibility is what turns a small grind error into a big hole. This is the standard screw machine and Swiss answer, where the drill often works right at the guide bushing on a rigid gang slide and holds location that a hanging jobber drill never could. If a hole matters and keeps misbehaving, guide the drill before you buy a better one.

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 beyond the normal couple thousandths means grind or runout, bellmouth means flex at entry, taper means corner wear or entry deflection, 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. Standards referenced: ANSI/ASME B94.11M (twist drills), plus published drill oversize data.