What Is Reaming? Reamed Holes Explained
The finishing pass that turns a drilled hole into a precise, round bore — tolerance, surface finish, stock allowance, reamer types, and how it compares to boring and honing.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 8 min read
On this page
Quick Answer
Reaming is the finishing pass after drilling that brings a hole to its final size, roundness, and surface finish. It removes only about 0.10–0.30 mm on diameter, typically achieves an H7 fit (IT6–IT8) and Ra 0.8–1.6 µm, and is the standard way to make precise bores for dowel pins, locating holes, and bearing seats. Reaming refines an existing hole; boring corrects size and location; honing gives the finest possible finish.
The Finishing Pass for Holes
A drill makes a hole; a reamer makes it precise. Reaming is a finishing operation that follows drilling, using a multi-flute cutting tool to remove a small amount of stock from an already-drilled hole. Its job is threefold: bring the hole to final size, improve its roundness, and improve its surface finish. You choose reaming when a drilled hole is already close to size and needs a tight fit — not when the hole needs major size correction, which is boring’s job. Understanding reaming is how you know what "H7" on a drawing actually costs to produce.
Reaming vs Boring vs Honing
The four ways to put a hole in metal, and what each one delivers. On round stock the hole usually starts on a lathe — see the CNC turning overview for when turning beats milling — and the full routing logic sits in our drilling vs boring vs reaming guide:
| Operation | Tolerance (IT) | Surface finish (Ra) | Role |
|---|---|---|---|
| Drilling | IT10–IT12 | 3.2–12.5 µm | Rough hole creation |
| Reaming | IT6–IT8 | 0.8–3.2 µm | Final size + roundness + finish |
| Boring | IT6–IT9 | 0.4–6.3 µm | Correct size and location flexibly |
| Honing | IT5–IT7 | 0.05–0.8 µm | Finest geometry and surface |
The pattern is simple: drilling creates the hole roughly, reaming refines size and finish, boring corrects size and location, and honing delivers the finest geometry and surface. Most precise bores are drilled, then reamed (or bored), and only honed when the tolerance demands it.
Tolerance and Surface Finish: What Reaming Achieves
A reamed hole typically achieves an H7-class fit, with common tolerances in the IT6–IT8 range — roughly ±0.01–0.025 mm depending on tool, material, and setup. The surface finish lands around Ra 0.8–1.6 µm, with 1.6 µm the everyday standard and 0.8 µm achievable in good conditions. Those numbers are why reaming is the default for dowel pins, locating holes, and bearing seats — features where a drilled hole is simply too rough and too sloppy. For the tolerance language behind H7 and IT grades, see our machining tolerances guide. One caution on finish callouts: those are Ra numbers, and a drawing that specifies Rz is working from a different scale — Ra vs Rz explains how the two relate.
Stock Allowance: A Tiny, Critical Number
Reaming is a light cut, and the amount you leave for it matters more than people expect. A common allowance is 0.10–0.30 mm total on diameter (0.05–0.15 mm per side), with smaller holes and harder materials toward the low end. Leave too much and you overload the reamer — oversize holes and chatter. Leave too little and the reamer cannot clean up the drilling marks, leaving a poor surface. This is why drill size selection for a reamed hole is not "nominal minus a guess" but a calculated step.
The band above covers the mid-size holes where most reaming happens. Across the full size range the allowance scales with diameter — roughly 2–3% of it — which is what a pre-ream drill chart is really encoding:
| Hole Ø range | Total stock on diameter | Working rule |
|---|---|---|
| Up to 3 mm | 0.05–0.10 mm | micro-drills wander; keep the reamer lightly loaded |
| 3–6 mm | 0.10–0.15 mm | ≈ 2–3% of diameter |
| 6–12 mm | 0.15–0.25 mm | ≈ 2–3% of diameter |
| 12–30 mm | 0.25–0.40 mm | toward the 2% end as diameter grows |
| Over 30 mm | 0.40–0.50 mm | reamers get costly here; boring takes over |
Reamer Types and the Classic Problems
Reamers come in several forms: hand reamers for manual finishing and repair, machine reamers for production, straight-flute and helical-flute designs (helical helps in tougher or deeper holes like stainless), and adjustable reamers for non-standard sizes. The three classic problems are oversize holes, chatter, and bellmouth (a flared entrance or exit). Almost all of them trace back to the stock allowance being wrong or the setup lacking rigidity — which is why reaming is a process-control exercise, not just a tool choice. At the forgiving end of the material list, machining brass is about as easy as reaming gets — it cuts clean, holds size, and rarely chatters.
When to Spec a Reamed Hole
Spec reaming when the hole needs a close fit — dowel pins, locating holes, bearing seats, or any bore with a tolerance tighter than a drill can hold. If the drawing calls out H7 or a ±0.01–0.025 mm bore, that is a reamed (or bored) hole, not a drilled one. Drilled holes are fine for clearance and non-critical passages, but the moment a pin has to locate or a shaft has to run, reaming enters the conversation. Our quality control guide covers how the final bore gets verified, and our GD&T symbols guide covers how position and runout callouts interact with the hole itself.
For the fits those precision bores create, see our engineering fits guide and press fit guide.
FAQ
What is reaming in machining?
Reaming is a finishing operation that follows drilling. A reamer — a multi-flute cutting tool — removes a small amount of stock from an already-drilled hole to bring it to its final size, improve roundness, and improve surface finish. Drilling establishes the rough hole; reaming does the final, controlled sizing pass. It is chosen when the hole is already close to size and needs a tight fit, not when major size correction is needed.
What tolerance can a reamed hole achieve?
A reamed hole typically achieves an H7-class fit, with common tolerances in the IT6–IT8 range — roughly ±0.01–0.025 mm depending on the tool, material, and setup. The surface finish is typically Ra 0.8–1.6 µm, with 1.6 µm the common standard and 0.8 µm achievable in good conditions. The exact numbers depend heavily on machine rigidity, hole size, material, and reamer type.
How much stock should be left for reaming?
Very little — a reamer removes only the last few tenths of a millimeter. A common allowance is about 0.10–0.30 mm total on diameter (roughly 0.05–0.15 mm per side), with smaller holes and harder materials toward the low end. Leave too much and you overload the reamer, causing oversize holes and chatter; leave too little and the reamer cannot clean up the drilling marks.
Reaming vs boring vs honing — what is the difference?
They refine a hole to different degrees. Reaming mainly improves size and finish on an already-correct hole. Boring corrects size and location more flexibly and can improve geometry. Honing is the finest finishing step, giving the best geometry and surface finish. In capability terms: reaming hits IT6–IT8, boring IT6–IT9, and honing IT5–IT7 with Ra down to 0.05 µm.
What are the common reaming problems?
The three classic ones are oversize holes, chatter, and bellmouth (a flared opening at the hole entrance or exit). Oversize and chatter usually trace to leaving too much stock, which overloads the tool and degrades size control. Too little stock is also a problem, because the reamer may not clean up the prior tool marks. The fix is dialing the stock allowance and keeping the setup rigid.
When should I specify a reamed hole instead of just a drilled one?
Specify reaming when the hole needs a close fit — dowel pins, locating holes, bearing seats, or any bore with a tolerance tighter than a drill can hold. If the drawing calls out H7 or a ±0.01–0.025 mm bore, that is a reamed (or bored) hole, not a drilled one. Our machining tolerances guide covers the tolerance side, and our quality control guide covers how the result gets verified.
Can you ream a hole with a drill bit?
Not with any control over the result. A twist drill dropped into an existing hole cuts on its margins and corners instead of its lips — it grabs, chatters, and follows its own idea of where the hole should go. What a drill bit cannot do is what a reamer is built for: take a light, even cut on every flute at once and leave a round hole at a repeatable size. A drill can rough the hole to near size; the last tenth of a millimeter belongs to the reamer.
Does reaming correct hole position or angle?
No — and this is the most expensive misconception in hole making. A reamer follows the hole it is fed into. It improves size, roundness, and surface finish, but the axis it cuts on is the axis the drill left behind: if the drilled hole is tilted or off-position, the reamed hole is precisely, beautifully tilted or off-position. Correcting position or angle takes a single-point tool that can walk the axis — that is boring.
What speed and feed should a reamer run at?
Slower than drilling, feeding harder than drilling. The standing rule is one-half to two-thirds of the drilling surface speed, with a feed rate two to three times higher — the many flutes share a light depth of cut, and a healthy feed keeps them cutting instead of rubbing and burnishing the wall, which work-hardens it and wrecks size control. Cutting fluid matters as much as either number. Start from the tool maker’s chart for the material and use those ratios as the sanity check.
Related Resources
What Is CNC Machining?
What is CNC machining? A plain-English guide to how it works, the main process types, materials, tolerances, and…
How Does CNC Machining Work? A Step-by-Step Look at the Process
How does CNC machining work? Follow a part from CAD to CAM, setup, machining, inspection, and shipping — and see…
Types of CNC Machining: Every Process and When to Use It
The main types of CNC machining explained: 3/4/5-axis milling, turning, mill-turn, Swiss machining, EDM, grinding —…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Sources
Standards and references behind the numbers on this page.
- Kennametal, Reaming Tool Basics and Tips — pre-ream hole sizing, and the speed and feed rules (one-half to two-thirds of drilling speed, two to three times the feed)
- Reamer — Wikipedia — reamer types and the stock-allowance concept
Holes Drilled, Reamed, and Inspected
IsoCNC drills, reams, and bores precise holes every day — dowel fits, locating bores, and bearing seats — verified on a CMM. Send the drawing; an engineer reviews every RFQ, typically within 1–2 business days.