Reaming for Precision Holes: Tolerances and Practice
Short answer: a drilled hole typically lands within ±0.05–0.1 mm, which is not good enough for a dowel pin or a bearing fit. Reaming removes the last 0.1–0.3 mm with a multi-edge cutter and produces an H7-class hole, for example 10.000–10.015 mm on a nominal 10 mm bore, with a finish around Ra 0.4–1.6 µm. Reaming fixes size, roundness and finish, but it does not fix position — hole location is set by the pilot drill. Use reaming for fits, boring for large or corrected holes, and drilling alone only where size is not critical.
Holes are the most common feature on machined parts, and they are also the feature most often specified loosely and made inconsistently. A hole that is drilled only is fine for a clearance bolt, but a hole that receives a dowel pin, a bearing or a press-fit bushing lives or dies on a few microns. Reaming is the standard, economical way to hit that window, and understanding its limits saves both money and scrap.
What Reaming Actually Does
Reaming is a finishing operation. A reamer is a straight or helical-fluted multi-edge cutter that is fed into a pre-drilled hole and removes a thin layer of material from the wall, sizing the hole and improving its roundness and finish. Because the reamer has many cutting edges that all contact the wall at once, radial forces largely cancel and the tool self-centres in the hole. The result is a hole that is round, straight and sized to the reamer, with a finish far better than a drill can leave.
The crucial limit is that a reamer follows the existing hole. It does not move the hole's axis. If the pilot hole is off-centre, the reamed hole is off-centre too, just rounder and better finished. This is why reaming is a sizing and finishing operation, not a locating operation.
Reaming also has a natural size ceiling. Because the hole ends up at the reamer's diameter, a shop needs a reamer in that size, and standard reamers come in standard steps and standard fits. If your drawing calls for an unusual nominal size or a very tight non-standard window, an adjustable reamer or a boring operation may be the practical answer. This is one reason to specify standard fits such as H7 wherever the application allows, because standard fits match standard tooling and standard tooling is faster and cheaper.
Drilling vs Reaming vs Boring
| Method | Typical hole tolerance | Surface finish | Corrects position? |
|---|---|---|---|
| Drilling only | ±0.05–0.1 mm | Ra 3.2–12.5 µm | Sets position |
| Drill + ream | H7 to H8 | Ra 0.4–1.6 µm | No |
| Drill + bore | ±0.01–0.02 mm | Ra 0.8–1.6 µm | Partly, if single-point |
| Boring on a lathe/mill | ±0.005–0.01 mm | Ra 0.4–1.6 µm | Yes, with setup care |
| Circular milling | ±0.02–0.05 mm | Ra 1.6–3.2 µm | Yes |
The table shows the trade clearly. Drilling is fast and sets position. Reaming takes that hole and makes it accurate in size and roundness but cannot move it. Boring can correct position and size because a single-point tool is adjustable and the machine controls its path, but it is slower and needs more skill. Circular milling is flexible but rarely as round or as accurate as reaming.
Reamer Types and Where Each Fits
| Reamer type | Use | Notes |
|---|---|---|
| Chucking (machine) reamer | CNC production | Standard for milled/lathe holes |
| Hand reamer | Low volume, repair | Long taper lead, turned by hand |
| Floating reamer | Compensates misalignment | Holder floats to follow the hole |
| Adjustable (expandable) reamer | Fine size control | Can be set to a target size |
| Shell reamer | Large diameters | Replaceable cutting head |
| Taper-pin reamer | Tapered pin holes | Matches a specific taper |
For CNC production the chucking reamer is the workhorse. A floating holder is useful when the reamer and the hole may not be perfectly aligned, because it lets the reamer follow the existing hole rather than fighting it. An adjustable reamer is the tool of choice when a shop needs to hit a specific size across a batch and wants to dial the tool in.
Preparing the Pilot Hole
The pilot hole decides whether reaming succeeds. Leave too little stock and the reamer rubs and dulls; leave too much and the reamer cuts unevenly and may chatter. A practical rule is to leave about 1–3% of the hole diameter as reaming stock, which for a 10 mm hole is roughly 0.1–0.3 mm on diameter. The pilot hole should also be drilled accurately, because its position becomes the reamed hole's position.
Pilot hole quality matters as much as its size. A pilot that is drilled with a worn bit, or that is bell-mouthed at the entry, will not guide the reamer well and the reamed hole may taper at the top. For critical holes, a spot drill followed by a rigid, sharp pilot drill gives the reamer the best chance of producing a straight, round result.
Speeds, Feeds and Setup Practice
Reaming runs slower and feeds faster than drilling, because the tool has many edges and does not need to plunge efficiently. Cutting speed is typically lower than drilling to avoid chatter and to protect the fine edges of the reamer, while feed per revolution is higher so the reamer cuts rather than burnishes. Coolant or cutting oil is important, because reaming produces fine chips that must be flushed away; trapped chips are a leading cause of scored holes and oversize results. A reamer should be fed steadily and never run backwards, which can dull or chip the edges.
Tool condition is decisive. A dull reamer cuts oversize, and an oversize hole cannot be recovered by reaming again with the same tool. Shops that hold tight H7 windows replace or inspect reamers on a schedule rather than running them until they fail. If a run starts producing holes at the top of the tolerance band and drifting, the reamer is usually the first suspect.
When Reaming Is the Wrong Choice
Reaming is wrong when position must be corrected, because it cannot move the hole. It is wrong for interrupted holes or cross-drilled holes, because the interrupted cut damages the reamer edges and spoils roundness. It is wrong for very large holes, where boring or circular milling is more practical. And it is wrong for blind holes that need a flat bottom, because a reamer usually has a chamfered lead that cannot produce a sharp internal corner. Recognising these cases early avoids a tooling cost that will not solve the problem.
Design Rules for Reamed Holes
Call out a standard fit rather than an arbitrary size — H7 for a tight locating hole, H8 where a little clearance is acceptable — because standard fits let the shop choose a standard reamer. Keep the hole depth within reach of a standard tool, and avoid specifying a reamed through-hole where a milled bore with a controlled position would be cheaper. State the function of the hole: a dowel pin, a bearing seat and a clearance hole each want a different tolerance, and quoting them all the same is either wasteful or unsafe.
It also helps to say whether the hole is through or blind, and whether it is cross-drilled by another feature. A through-hole is easier to ream and to flush clean; a blind hole traps chips and needs care. A hole crossed by another drilling is an interrupted cut that damages a reamer, so that hole may need boring instead. These details rarely appear in a quick enquiry, yet they decide the process, and giving them up front leads to a quote you can trust rather than one that gets revised after the parts are cut.
Frequently Asked Questions
Q: What tolerance can reaming hold?
A: A reamed hole typically lands in the H7–H8 range, so on a 10 mm nominal bore that is roughly 10.000–10.015 mm for H7. It also gives good roundness and a finish around Ra 0.4–1.6 µm. It does not improve the hole's position, which is set by the pilot drill.
Q: Does reaming fix an off-centre hole?
A: No. A reamer follows the existing hole, so it makes the hole rounder, better finished and correct in size, but it cannot move the axis. If position matters, the pilot hole must be made accurately, or the hole should be bored so the machine can correct its path.
Q: How much material should be left for reaming?
A: Roughly 1–3% of the hole diameter, which is about 0.1–0.3 mm on diameter for a typical hole. Too little stock and the reamer rubs and dulls; too much and it cuts unevenly and may chatter. The pilot hole should also be straight and accurately positioned.
Q: How many edges does a reamer have, and why does that matter?
A: A reamer has several cutting edges rather than the two of a drill, and they contact the wall together, so radial forces largely cancel and the tool self-centres. That is why the resulting hole is round and well sized even though the reamer is a finishing tool that follows the pilot hole rather than steering it.
Q: When should I bore a hole instead of reaming it?
A: Bore when the hole is large, when its position must be corrected, or when you need a tighter tolerance than H7 or a specific size that no standard reamer gives. Boring is slower but the machine controls the path, so it can fix location as well as size. Send us the drawing and we will quote the right route.
Related Resources
- How holes are made: drilling, boring, reaming and EDM — the full menu of hole-making options and how to choose.
- CNC machining services — precision hole work and machining from a Dongguan source factory.
- About BQUQ — an ISO9001 source factory running CNC, stamping, spring and heat sink lines under one roof.
- Contact us — send your drawing for a quote within 12 working hours.
Authored by the BQUQ Engineering Team. BQUQ is an ISO9001-certified source factory in Dongguan, China, running CNC machining, metal stamping, custom springs, heat sink and collet lines under one roof. Send drawings to sc@bquq.com or WhatsApp +86 13713157787 for a quote within 12 working hours. www.bquq.com
