A drill makes a hole, but it does not make a hole to size. Twist drills routinely cut oversize, wander off center, and leave a wall that looks torn under magnification, so a hole that must take a dowel pin, a bearing, or a locator usually needs a second, finishing step. Reaming is that step. A reamer is a multi-fluted finishing tool that takes a small, even cut from a drilled or bored hole and leaves it round, straight, and sized to a tolerance a drill can never hold. It is one of the cheapest ways in machining to turn an "almost right" hole into a "right" one, and it fails in predictable, avoidable ways.
What a reamer does that a drill does not
A drill is a two-flute plunging tool that removes most of its material from the center outward and is guided only by its own rigidity and the cut it is making. It is built to remove stock fast, not to produce a precise bore. The reasons are structural. A drill has only two cutting edges doing all the work, and if the two edges are even slightly unequal in length or angle, the drill pulls sideways, walks, and cuts a hole that is larger than its nominal size and not perfectly round or straight. The point of the drill also has no support, so a drill starting on an uneven or angled surface tends to skid before it bites.
A reamer works on the opposite principle. It has an even number of flutes, usually six or eight for a finishing reamer, arranged evenly around the circumference, and each flute takes a very light cut. Because the load is spread over many edges and the reamer is guided by the hole it is already inside, it cannot wander the way a drill can. It straightens and trues the hole, removes the torn surface the drill left, and brings the diameter up to a tight tolerance with a much finer finish than drilling alone can produce. The reamer is not doing the heavy work; it is correcting what the heavy work did.
The cost of this is that a reamer cannot start a hole. It has no point and no ability to plunge into solid material, so it must always be preceded by a drill or a boring operation that leaves a hole slightly undersize and close enough to true that the reamer only has to clean it up. This "stock allowance" is the single most important number in reaming, and getting it wrong ruins the hole no matter how good the reamer is.
The stock allowance: the number that makes or breaks the hole
The stock allowance is the amount of material the reamer removes, expressed as the difference between the pre-ream hole diameter and the finished diameter. It is small on purpose. A finishing reamer is meant to take a light, even cut, and the allowance is typically a few hundredths of a millimeter in total, split across the flutes. Too much stock, and the reamer is forced to do a drilling job it was not designed for; the flutes overload, the hole comes out oversize and bell-mouthed, and the surface finish degrades. Too little stock, and the reamer has nothing to bite into, so it rubs instead of cuts, work-hardens the wall in tougher materials, and produces a glazed, torn finish rather than a clean one.
The right allowance scales with the hole size and the material. A small hole in aluminum might take a total allowance of around a tenth of a millimeter on the diameter, while a larger hole in stainless or a hard steel needs more so the reamer is actually cutting rather than burnishing. The key is that the allowance be consistent from hole to hole, which is why the drill size that precedes the reamer is chosen deliberately. There is a standard progression of drill sizes that leave the right amount of material for each finished reamer size, and the machinist picks that drill rather than whatever happens to be in the rack.
| Fault | Usual cause | What it does to the hole |
|---|---|---|
| Oversize hole | Excess stock allowance or misalignment | Reamer overloads, bell-mouths the entry |
| Bell-mouthed entry | Reamer not aligned to the hole axis | Entry is larger than the rest of the bore |
| Torn or glazed finish | Too little stock, rubbing instead of cutting | Work-hardened wall, poor surface |
| Out-of-round bore | Uneven stock from an off-center drill | Reamer follows the bad hole instead of fixing it |
| Chatter marks | Excess speed or a worn, dull reamer | Ridged wall, noisy cut |
| Undersize hole | Worn reamer cutting below nominal | Pin or bearing will not seat |
Speed, feed, and why reaming runs slow
Reaming runs at a fraction of the speed and a higher feed than drilling, and the reasons follow directly from what the tool is doing. A reamer has many edges taking a tiny cut, and each edge needs time to cut cleanly rather than to skid. The spindle speed is typically run at about one-third to one-half of the speed used for drilling the same material, and the feed is set higher per revolution so the tool advances steadily and each flute shaves its share of material instead of rubbing. The result is a steady, deliberate pass that produces a smooth, continuous chip — a thin, springy curl that looks nothing like the short, thick chips a drill throws.
The single most common mistake in reaming is running too fast. A reamer that spins too fast vibrates, chatters, and leaves a ridged wall instead of a smooth bore, and because the tool has so many edges, a tiny imbalance or a slightly worn flute is amplified into a visible finish defect. The second mistake is feeding too slowly, which lets the reamer rub instead of cut and burns the edge. The right combination feels and sounds unhurried: a low, steady note, a light load, and a fine, continuous chip coming off every flute.
Coolant matters here more than in drilling, because the cut is light and the tool dwells in the hole. A steady flood of cutting fluid washes the fine chips out of the flutes and keeps the edge cool and lubricated, which is what lets a reamer hold size across a long run. A reamer that runs dry or with an intermittent coolant hit will gall, load its flutes, and cut oversize. This is also why reaming is usually done as a separate, dedicated operation rather than squeezed into a drilling cycle, so the speed, feed, and coolant can be set for the reamer alone.
Alignment, and why it decides the whole operation
The reamer's greatest strength is also its greatest vulnerability: because it is guided by the hole, it follows the hole. If the drilled hole is off-center, angled, or bell-mouthed, the reamer faithfully straightens what it can but cannot move the axis of a badly placed hole. A reamer will correct a hole that is slightly oversize or slightly torn, but it will not relocate a hole that was started in the wrong place, and it will not fix a hole whose axis is tilted relative to the face. The position and the angle are set by the drill — and by the spotting operation that should precede it — not by the reamer.
This is why precise hole-making is a sequence, not a single tool. A proper routine starts with a center drill or a spot drill that puts a short, accurate starting cone exactly where the hole belongs. The twist drill then follows that cone and stays on the intended axis. Only after the hole is roughly to size and on location does the reamer come in to finish the diameter and the surface. Skipping the spotting step and going straight in with a drill is the fastest way to get an off-center hole that no reamer can save.
On a CNC machine, the reamer must also be aligned with the spindle and run true, because a reamer held slightly off-axis will cut a hole larger than its nominal size and bell-mouth the entry. This is why reamers are often run in a floating holder or a holder that allows a little self-alignment, letting the tool center itself in the hole rather than fighting the spindle. The same logic applies to the workholding: the part must be held so the hole axis is stable and square, because a reamer cannot compensate for a part that flexes or a fixture that lets the hole move.
Where reaming fits, and where boring takes over
Reaming is the workhorse for holes that are small to medium in diameter, relatively shallow, and need a tight tolerance plus a good finish at low cost. Dowel-pin holes, locator holes, guide-pin bores, and bearing seats are the classic cases, and in aluminum or mild steel a reamed hole can hold a tolerance on the order of an H7 or H8 fit without a great deal of fuss. The tool is inexpensive, the cycle time is short, and the process is forgiving of ordinary shop conditions, which is why it is the default choice whenever a hole has to fit a standard pin or a bushing.
It is not the right tool for every hole. For large diameters, deep holes, or interrupted cuts, reaming becomes unreliable, and boring is the better answer. A boring bar can be adjusted to hit a diameter exactly, corrects a hole's position and straightness in a way a reamer cannot, and works at any size above a modest minimum. The trade is that boring is slower and requires more skill and a more rigid setup, so it tends to win on the holes where precision and position matter most, while reaming wins on the everyday holes where a standard pin has to slide in cleanly and stay put.
- Leave the right stock allowance — a few hundredths of a millimeter, more for larger or harder holes.
- Spot or center-drill first — the drill only stays on axis if it starts on axis.
- Run slow and feed steady — about one-third to half the drilling speed, higher feed per rev.
- Keep coolant flooding — a light cut dwelling in the hole needs washing and lubrication.
- Hold the reamer true — a floating holder lets it self-center instead of fighting the spindle.
- Let the reamer follow the hole — it finishes size and finish, it does not relocate a bad hole.
- Watch for bell-mouthing — the first sign of too much stock or a misaligned entry.
- Switch to boring when reaming can't hold it — large, deep, or position-critical holes.
"Reaming is a correction step, not a locating step. Get the hole started on axis with a spot drill, drill it roughly to size, and then let the reamer do the one thing it is good at: shaving a few hundredths off the wall so the hole is round, straight, and sized for the pin that has to slide into it. Skip the spotting, load the stock wrong, or spin it too fast, and no reamer on the shelf will save you."
When a hole has to take a dowel pin or a bearing, the difference between a drilled hole and a reamed one is the difference between a press fit and a fight. Set the stock allowance, start the hole on axis, run the reamer slow and flooded, and the hole comes out round and to size at a cost that is hard to beat anywhere else in the shop.
If your drawings call for dowel-pin holes, locators, or bearing bores that keep coming back oversize or torn, send them over and we will review the stock allowance, the drill sequence, and the numbers behind the hole. See how we approach CNC milling for precision bores and turned parts with tight bores, or get a quote on your part.