Drilling vs Boring vs Reaming: Which Hole Process
Almost every machined part has holes, and almost every hole question comes down to the same three processes. This guide separates them by what each one does to the hole — stock removed, tolerance, finish, and whether position can be corrected — so your drawings route holes the way a shop would.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 14 min read
Quick Answer
Drilling makes the hole exist, and it makes it fast and rough: IT12–IT13, feed marks you can feel, and wherever the drill felt like wandering that day. Boring is the only one of the three that can fix where the hole ended up — a single-point tool at an adjustable radius, ±0.05 mm on a normal day, IT5 with a finish head. Reaming is the last pass: a multi-flute tool that removes a deliberate 0.05–0.25 mm and lands the hole on its fit band, H7 as routine, Ra 0.8 µm common.
Route holes by what the drawing demands: drill for most of them, ream for the ones that locate things, bore in the middle when position or size has gone wrong — and hone past all of it when the drawing gets serious.
The Hole You Drilled Is Not the Hole on Your Drawing
Every machinist learns this eventually, usually at the worst possible moment. The drill gave you a hole, yes — but it’s oval-ish, 0.1–0.2 mm oversize, tilted a fraction of a degree, and sitting 0.1 mm off where you programmed it. None of that is the drill’s fault. A twist drill is a long, flexible tool that cuts with its whole body; asking it to produce a round, straight, accurately placed hole is asking a screwdriver to finish a chisel’s job.
So hole work is a chain, and each link exists because of the one before it. Drill gets you existence. Bore — only when needed — gets you truth: position, roundness, size. Ream gets you the fit: final diameter and finish. Hone is the step after reaming, for bores that need to be genuinely round and genuinely smooth. Most holes never leave the drill, and that’s correct — every step past it costs machine time, so the discipline is buying exactly as many steps as the drawing pays for.
Vocabulary note before we go further: blind vs through holes matters here more than you’d think — a blind hole changes your reamer choice and your chip situation — and the flat seats that usually surround a finished hole live in our counterbore vs spotface breakdownur counterbore vs spotface guide.
What Drilling Is Actually Good At
Speed and existence. A twist drill — fluted to move chips, point angle ground for the material — plunges into solid stock and takes the hole with it in seconds. On a CNC mill you spot-drill first with something short and stiff so the point has a pocket to start in, then peck-cycle your way down, and the machine just repeats it, hole after hole, all shift. As a material-removal process it’s close to unbeatable.
What it’s not good at is any of the qualities you associate with a finished hole. Diameter lands around IT12–IT13. The wall carries visible feed marks. Position inherits every micron the drill wandered, and it wanders because the tool is flexible and cutting with its whole length. This is all fine — a clearance hole for a bolt couldn’t care less. The failure mode is writing H7 on a drilled hole and hoping. That’s not a challenge for the shop; it’s a routing error on the drawing, and the shop will either quietly add processes and charge you, or quote it as-is and deliver a surprise.
Boring: the One That Fixes Position
If you remember one thing about boring, remember this: it’s the only process in this article that can move a hole. A boring bar is a single-point tool on an adjustable radius — on a lathe the part spins, in a mill’s boring head the tool spins. Either way, the bar cuts a circle that is concentric with the spindle, period. It doesn’t care where the drilled hole drifted; it opens that hole out and puts the finished circle where the program says.
It does the rest well too. Diameter: ±0.05 mm is a normal day, and a finish boring head will reach into IT5 territory. Form: roundness and straightness improve as a matter of course, and with care you’re holding cylindricity as a callout. The classic trade against reaming is that boring wins geometry and reaming wins finish — and for holes from roughly Ø20 up, boring is also the economical answer, because a bar and one insert cover a range of sizes while reamers are bought one diameter at a time.
The fair question on a modern CNC machine: why not helical-interpolate the hole with an end mill? For a lot of work you can, and shops do. But the boring bar still cuts the rounder circle — the spindle’s bearings define it, not servo moves — and it still takes the better finish at tight grades. Below about Ø20 the bar gets unwieldy and interpolation or reaming takes over.
Reaming: the Last Pass
Reaming is deliberately boring. The hole already exists, close to size, and the reamer — multi-flute, fixed diameter — removes a small planned amount and stops. That amount is smaller than people guess: 0.05–0.15 mm on diameter for finishing, up to 0.25 for a roughing pass, or the shop rule of 2–3% of the reamer’s diameter. For reamers under 10 mm, plan on about 0.10 mm of stock.
Why bother for so little material? Because what comes out the other side is a hole you can build on. Many flutes sharing a tiny cut means a finish nothing earlier in the chain touches — Ra 0.8 µm is routine, 0.2 with care — and diameter consistency good enough that H7 reamers are catalog items. You call the band, the reamer makes the band.
The catch is the reamer’s personality: it’s a follower. Guided by the hole it’s in, it goes where the pre-hole goes and makes it shinier. Ream a hole that drifted and you get a beautiful hole in the wrong place — which is the entire reason boring exists upstream. The reaming guide has reamer types and stock allowances in detail.
The Three, Side by Side
Same machine, same part, three different jobs. The table is the honest version of the division of labor.
| Attribute | Drilling | Boring | Reaming |
|---|---|---|---|
| What it does | Makes the hole from solid | Enlarges and true-ups an existing hole | Finishes an existing hole to size |
| Material removed | Large — the whole hole | Medium to large, adjustable | Tiny — 0.05–0.25 mm on the diameter |
| Typical tolerance | IT12–IT13 (loose) | ≈±0.05 mm; finish boring reaches IT5 | IT6–IT9, routinely H7 |
| Surface finish | Rough, visible feed marks | Smoother than drilling; finish boring better than Ra 1 µm | Ra 0.8 µm routine, down to 0.2 µm |
| Corrects hole position | No — the drill wanders with it | Yes — the defining advantage | No — follows the existing hole |
| Tool | Twist drill (multi-flute) | Single-point boring bar | Multi-flute reamer |
| Role in the chain | Always first | Middle — when position or roundness must move | Last machining step before honing |
Read the position row twice — it’s the one that decides your routing. Position doesn’t matter? Drill and ream, done. Position matters, and the drawing ties the hole to datums the way GD&T position callouts do? Now boring is in the chain, before the reamer — or the reamer is just polishing an error.
Routing by What the Drawing Says
Shops don’t pick these processes from mood. They read the callout and run the route it implies — six situations cover nearly everything:
| Drawing callout | Route | Why |
|---|---|---|
| Ø10 general, ±0.13 mm | Drill only | Tolerance and finish non-critical — the drill hole is already good enough |
| Ø10 H7, position free | Drill undersize + ream | The reamer makes the H7 band directly; position inherited from drilling is acceptable |
| Ø10 H7, tight position to datums | Drill + bore + ream | Boring first moves the hole onto true position; the reamer then finishes to size |
| Ø40 H7 | Drill + bore (finish) | Large reamers are costly and torque-hungry; a finish boring head reaches the grade and holds position |
| Ø8 H7, deep, roundness critical | Drill + bore + ream + hone | Honing takes roundness and finish beyond what any blade or flute can hold |
| Ø0.8 mm deep hole | Gun drill | A twist drill packs its chips and loses the hole at depth; the gun drill was built for it |
Behind the table, two economics. Time: a drilled hole is minutes; boring and reaming each add another operation on the same hole; honing is a step again — which is why tolerance generosity on holes that don’t function is the cheapest DFM you’ll ever do (the DFM guide beats this drum properly). Tooling: drills come in every size, reamers get bought per size and wait in a drawer, one boring bar covers a range — big precision holes bore, small ones ream, and it’s not tradition, it’s the tool crib.
Deep Holes Change the Rules
Past a depth-to-diameter ratio of 3–5, the twist drill starts living on its flute length. Chips pack the flutes, coolant can’t reach the point, the drill walks harder, straightness goes soft. The answer is gun drilling: one cutting edge, straight flutes, coolant through the tool, one pass with a guide bushing — straightness at depth-to-diameter ratios past 20:1, territory a twist drill wouldn’t attempt. Cross-holes in long shafts and oil passages in hydraulic manifolds are its natural work.
On the finishing end, deep-and-small is exactly where honing earns its keep — the process this shop does its best work in. A deep hole whose roundness and finish matter more than its position can skip the reamer entirely: drill or gun drill, then hone. Add a boring pass in between only if position matters too. And the same instinct sorts ordinary holes — clearance holes for fasteners die happily as-drilled, while dowel holes go the whole way to the reamer.
Mistakes, and What Each One Costs
Calling a drilled hole H7. The drill won’t, so either the shop quietly adds a reamer and bills it, or quotes the drawing literally and ships you IT12 with a straight face. Write the band you actually need; let the routing happen on the shop side where it belongs.
Wrong reaming allowance. Too little stock and the reamer burnishes and comes up under size; too much and it deflects, chatters, and bells the mouth. The 2–3% guideline is the reamer telling you it wants to cut, not rub.
Skipping bore on a position-critical pattern. A reamed hole in the wrong place passes every diameter check and fails every assembly. The classic do-nothing-everything-checks-out nonconformance.
Boring thin walls with no support. The single-point cut pushes; thin sections spring away and the bore pinches tight in the middle. Fixturing, or a light final pass, is the cure — knowing this one is the difference between someone who bores thin walls and someone who bores them well.
Checking only the diameter. A bore gauge tells you size and nothing else. Position, roundness at depth, bell-mouthing — that’s CMM work, and for holes that locate anything it’s the only report that counts. Our FAI guide shows what that report should contain.
FAQ: Drilling vs Boring vs Reaming
What is the difference between drilling and boring?
Drilling starts the hole from solid material; boring enlarges a hole that already exists. That's the whole difference, but it explains everything else. The drill is a long multi-flute tool that wanders, so the hole it leaves is rough, oversized-ish, and wherever it ended up. The boring bar is a single-point tool at an adjustable radius, so it controls diameter to ±0.05 mm and better, improves roundness, and — the part no other hole process can do — puts the hole back on position, because the bar cuts a circle concentric with the spindle no matter where the drilled hole drifted.
What is the difference between boring and reaming?
Both finish an existing hole, and they're good at opposite things. Reaming makes the better surface — Ra 0.8 µm is everyday work — and the more repeatable diameter, which is why H7 holes are usually reamed. But a reamer is a follower: it goes where the pre-hole goes. Boring holds or improves position, roundness, and straightness, sets any diameter you dial in, and with a finish head reaches IT5 — at the cost of a surface one step behind the reamer's. Geometry, bore. Size and finish, ream.
Can you ream a hole without drilling first?
No, and there's no trick around it — a reamer can't start a hole, it can only finish one. It's designed to remove a small known amount from a hole that's already close: roughly 0.05–0.15 mm for finishing, 0.15–0.25 for a roughing pass, or the shop rule of 2–3% of reamer diameter. Drill (and bore, if position matters) undersize by that much, then ream. Too little stock and the reamer burnishes instead of cutting; too much and it deflects and drags the hole out of round.
Which process gives the tightest tolerance?
Finish boring and reaming tie on paper and split the medals in practice. Reaming wins diameter consistency — H7 with an off-the-shelf tool, every day, which is why dowel and bearing-bolt holes are reamed. Finish boring with a good head reaches the tightest grades of the three (IT5) and is the only one that also tightens position. And past all three, if the drawing wants single-micron roundness or Ra 0.1 µm, the answer is honing — neither a flute nor a blade lives there. At IsoCNC we quote precision features to ±0.025 mm (±0.001 in) against the drawing and verify with bore gauges and CMM.
When do you need boring instead of just reaming?
Three situations. Position: the hole has to sit on datums — coaxial bores, a hole true to a machined face — and the drill's wander has to be corrected before anything finishes it; only boring corrects position. Size: large holes, say Ø40 and up, are usually bored because big reamers are expensive, torque-hungry, and one diameter forever. Flexibility: a boring bar is adjustable, so it absorbs springback and tool wear without anyone buying a new tool — which is exactly the economics you want in short-run work.
What comes after reaming for the finest finish?
Honing. Reaming lands Ra 0.8 µm routinely and about 0.2 at its best; when the drawing calls for mirror bores, single-micron roundness, or a controlled crosshatch — hydraulic bores, gear pump bodies, compressor cylinders — honing is the final step. Floating abrasive stones correct the last geometry errors while taking finish down to Ra 0.05–0.2 µm. Our honing guide covers the process in depth, and the reaming guide covers everything up to that line.
Related Resources
304 vs 316 Stainless Steel: Which Grade for Machined Parts?
304 vs 316 stainless steel compared for CNC machined parts: composition, corrosion resistance (PREN), machinability,…
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,…
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
Holes Routed Right, Finished to Band
IsoCNC drills, bores, reams, and hones holes to the callout — precision features to ±0.025 mm (±0.001 in) against the drawing, verified with bore gauges and CMM under first-article inspection. Send the drawing through our CNC machining services and an engineer will review hole routings with the quote, typically within 1–2 business days.