Reaming Holes: Precision Hole Machining

A drill is fast but inaccurate: it leaves a hole at IT11-IT13 tolerance, scored and slightly out of round. That is fine for a bolt, but not for a bushing fit or a dowel pin. Reaming is the hole-machining method that turns a drilled hole into a precise one: IT7-IT9 tolerance and a smooth wall. In this guide we explain how reaming differs from simply enlarging a hole with a bigger drill, how to choose the tool and its working parameters - and, as a bonus, what "drilling out a lock" really means at the locksmith's.

What reaming and core drilling actually do

Reaming is a chip-forming machining operation performed with a multi-edge tool - the reamer - which removes a small stock allowance from the walls of an existing hole. The goal is not to remove volume but to improve three things at once: diameter, geometry and surface finish. A well-run reaming process delivers dimensional and form accuracy of IT7-IT9 (fine reaming even IT6) and surface roughness of Ra 0.32-1.25 um - values drilling alone will never reach.

Core drilling (counterboring with a larger drill), by contrast, is enlarging a previously drilled hole with a bigger drill or a core drill. In a classic process plan these hole-machining operations form a ladder: drilling, core drilling, rough reaming and finish reaming. The higher you climb, the smaller the allowance and the better the hole quality.

It is worth sorting out the terms, because in shop language all three operations get called "reaming":

• Core drilling - enlarging the hole with a drill or core drill; it improves the position of the axis, but accuracy stays at IT10-IT12.
• Rough reaming - with a roughing reamer; prepares the hole for the finishing pass, IT8-IT10.
• Fine (finish) reaming - with a finishing reamer; final size and finish, IT6-IT8.

Reaming is thus the classic finishing operation for holes: it completes what the drill started. Where this stage sits in the process plan of a whole part is covered in our guide to finish machining - here we focus on holes only.

The reamer: design, types and geometry

A reamer looks like a drill that agreed to a compromise: more cutting edges (typically 4-12), smaller entering angles and a very shallow cut. It consists of a working part (cutting and calibrating sections), a neck and a shank. The chamfered cutting section removes the allowance; the calibrating section guides the tool in the hole, burnishes the wall and holds the size. That long calibrating section is what stabilises the hole walls and keeps the tool from "diving" into the material the way a drill does.

There are many types, sorted by a few divisions:

• Hand and machine reamers - hand reamers have a long cutting taper and a square shank for a tap wrench; machine reamers are shorter and run on drill presses, lathes and machining centres.
• Fixed and adjustable - adjustable reamers allow small diameter changes, handy for repair fits.
• Cylindrical and taper - taper reamers serve, among others, holes for taper pins and tool sockets.
• Straight and spiral flutes - spiral flutes handle keyways and interruptions in the hole better.

Two design details have non-obvious reasons. First, the edges are spaced around the circumference with an uneven pitch: if they were spaced perfectly evenly, vibration would print regular ridges into the wall. Second, for deep holes with high demands, single-edge reamers with carbide guide pads are used: the pads burnish the wall right behind the edge, so the tool is supported on the freshly machined surface. This solution comes from hydraulic cylinder technology.

A worn tool loses finish first, size second. Regrinding a reamer means resharpening the cutting section only - the calibrating section is usually left alone, because it is what "holds" the diameter. Once wear reaches the calibrating section, the tool is only good for a size one grade coarser.

Rough reaming and fine reaming

Splitting the reaming process into a rough and a fine pass is not bureaucracy - it follows from cutting physics. The tool cuts shallow, so it copes badly with large, uneven allowances: instead of cutting it starts to squeeze the material, and the hole comes out tapered or lobed. That is why the stock allowance is split into two passes:

The allowance for finish reaming must be small but not zero: below about 0.05 mm the edges stop cutting and merely rub, which destroys the finish instead of improving it. The depth of cut per edge is half the diametral allowance - with 0.2 mm on diameter, each edge removes a mere 0.1 mm. Such a small depth of cut also means small forces - which is why a slender tool can hold a straight axis at all.

The hole tolerance dictates the chain of operations. For IT9, drilling plus one reaming pass is enough; IT7 already needs both passes; and where IT6 and a mirror wall are required, honing or superfinishing follows the reaming. Getting accurate holes is always a sequence, never a single operation - which is why precise holes cost disproportionately more than plain drilled ones.

Remember that a reamer improves diameter and form but does not correct the position of the hole axis - it follows the existing hole. If the axis is bent after drilling, boring straightens it, not reaming. It is a classic handbook rule: first fix the position, then the size, and the wall finish last.

Reamer working parameters

Reamer working parameters follow a different logic than drilling parameters: cutting speed is low and feed is high. The low speed (for HSS in steel typically 4-12 m/min, for carbide 10-30 m/min) limits vibration and built-up edge, which instantly ruin the finish. The high feed rate (0.2-1 mm/rev, several times more than in drilling) sounds counterintuitive but has a reason: each edge cuts a thin layer, and too small a feed makes the edges slide over the material, work-hardening the hole wall.

Typical catalogue values for reaming structural steel with an HSS tool are vc = 6-10 m/min and f = 0.3-0.8 mm/rev; in cast iron, feeds can be even higher. Spindle speed is calculated from these values exactly as for any other tool - formulas and worked examples are in our article on the cutting parameters calculator. One practical rule from us: if the reamed hole is "smooth but striped", vibration is usually to blame - and lowering the RPM helps, not lowering the feed.

Cooling plays a huge role in the reaming process. Emulsion flushes away the fine chips that would otherwise score the walls and stabilises the temperature on which the size depends - and with it the entire wall finish. Coolant pressure matters especially in blind holes: too little pressure will not flush chips off the bottom and the tool starts pressing them into the wall. In through holes the coolant is directed to flow with the chip evacuation.

The material changes the numbers

Every material reams differently. Aluminium is forgiving but sticky: without sharp edges and emulsion it forms a built-up edge that oversizes the hole - but it tolerates speeds twice those of steel. Stainless steel work-hardens, so it demands a decisive, continuous feed; any hesitation leaves a hard, shiny zone the next edge skates over. Grey cast iron is often reamed dry or with an air blast - the graphite in its structure lubricates the edges, and emulsion would form an abrasive paste. Brass and bronzes are practically made for this operation: short chips, low forces, a size stable from the first part.

Springback differs too: the same tool diameter gives a slightly larger result in aluminium and a smaller one in titanium than in steel. That is why the first part after a material change is always treated as a trial part.

Manufacturers' recommendations for reaming holes are a starting point: the working parameters are corrected after the first parts, based on measured diameter and surface quality. How smoothness is described in numbers is covered in our guide to surface roughness Ra and Rz.

Photo from Unsplash

CNC reaming: precision in practice

On numerically controlled machines, reaming stops being a craft and becomes a repeatable cycle. CNC machines guide the reamer rigidly along the axis of the drilled hole, and a canned cycle (e.g. G85: entry at working feed, exit also at feed, without stopping the spindle) ensures the wall is not scored on retraction. Hole finishing happens in the same setup as drilling, so the re-clamping error disappears. Making precision holes starts long before the last tool - the CNC hole machining process usually looks like this: spot drill, precise pilot drilling, drilling to the pre-ream size, boring if needed, and the finishing pass last.

Precise pilot drilling before reaming is not overkill - the tool copies position errors. That is why for demanding holes the axis is established with a spot drill and a short, rigid drill before the main drill enters. The whole CNC cycle gets a dozen seconds longer, but it saves scrap.

Advantages of CNC reaming

The biggest advantage is repeatability: the hundredth hole has the same diameter as the first, because the result comes from tool geometry, not the operator's hand. Accurate holes stop depending on operator skill, and the wall finish comes straight from the edge geometry. Add predictable hole quality - a high surface quality with no polishing - and short cycle times: the finishing pass takes seconds. Compared with boring, reaming is faster and simpler to program; compared with internal grinding - cheaper and available on an ordinary machining centre. The limit is diameter: above roughly 40-50 mm the tools get expensive and give way to boring.

Applications of CNC reaming

CNC reaming is the standard wherever precision holes for fits are made: dowel pin holes in housings and mould plates, sliding and guide bushings, small bearing seats, piston pin bores, valve guides, holes in levers and linkages. Making precision holes this way pays off especially in series production: where boring would need a size correction every few parts, a reamer holds the size for hundreds of parts.

A good example is machining accurate dowel holes in injection mould plates: dozens of H7 holes in one part, all made with the same cycle on one CNC machine. Making those accurate holes any other way - boring each one individually - would stretch the process severalfold.

CNC reaming services and CNC hole machining

For CNC shops, making precision holes is daily bread, so reaming services are rarely bought separately - they are part of the larger whole that is CNC machining of holes in a finished part. Precise holes for fits do need to be ordered consciously, though. For the buyer one thing matters: mark clearly on the drawing which holes carry a fit tolerance (H7, H8) and which are "plain". Every toleranced hole is an extra operation and an extra tool, so it translates directly into price. In MetronQ you see this relationship instantly: upload the model and drawing to the instant CNC quote and the system shows how hole tolerances change the part cost.

The hole machining process at a subcontractor always looks similar: drill all the holes, then run the precision operations in order of decreasing demands. A well-planned process starts from the tightest tolerance on the drawing. The machining method is chosen to match the tolerance, the batch size and the available tools - reaming competes here with fine boring and honing, and the finishing of large-diameter bores is done with boring heads.

Through holes, blind holes and deep holes

Through holes are the most grateful ones for reaming: chips and coolant have somewhere to escape, and the calibrating section can exit the material. Machining through holes also allows tools with a long taper lead, which run more calmly. Blind holes require tools with a short lead and careful flushing of the bottom - this is where coolant pressure and direction make the biggest difference.

Deep holes are a league of their own. Conventionally they start where depth exceeds 5 diameters - and they can be through or blind; machining holes whose depth exceeds 10xD already requires special techniques. Deep hole drilling descends from gun barrel technology and from well drilling - hence the jargon in which "borehole" originally meant a hole in rock and today gets used for any deep cylindrical hole. Formally a borehole is still a mining term, but the techniques are shared: tool guidance and high-pressure cooling. In shop practice, deep cylindrical holes are drilled with gun drills fed with internal coolant, and reamed with single-edge tools with guide pads.

Scale matters in both directions. In general, drilling cylindrical holes for reaming always leaves an allowance for the next tool. Drilling small holes (under 3 mm) for reaming demands caution, because a slender tool snaps easily - feeds are halved. Drilling larger holes for reaming, in turn, is done in steps: a smaller drill first, then a bigger drill to size with allowance, so that no single tool takes too large a chip cross-section. A large-diameter drilled hole almost never comes out straight from a single drill - and accurate holes start precisely from a straight axis.

One more practical note: small through holes in thin walls tend to "breathe" after reaming - the material springs back and the diameter comes out smaller than the tool. An experienced process engineer then picks a tool 0.005-0.01 mm larger, or changes the clamping so the part is not squeezed around the hole.

Photo from Unsplash

How to drill out a lock cylinder

"Reaming" lives a second life in emergency locksmithing. When a key breaks or gets lost and the cylinder will not open, the locksmith "drills out the lock". Technically this is not reaming in the machining sense but destructive drilling: the goal is to drill through the pin line so the plug can be turned with a screwdriver. We cover it because the question comes up all the time - and the answer has a lot in common with hole technology.

A legal and practical caveat: drill only your own lock, and if the door has a certified anti-burglary cylinder (class C / grade 6), let it go - hardened rods and carbide pins will stop ordinary drills. Calling a locksmith is then cheaper than ruined door hardware.

Drilling out a lock cylinder step by step

1. Centre-punch the drilling point on the plug's parting line, about 2-3 mm above the edge - that is where the pins sit.
2. Start with a small drill (3 mm) for metal; low RPM, with oil. Precision matters more than force - this is, at heart, precise hole drilling in hardened steel.
3. Work along the whole pin line - you will feel characteristic "clicks" as the drill breaks successive springs and pins.
4. Enlarge the hole with a 4.5-6 mm drill. Doing it safely in two passes protects the drill from snapping inside the narrow cylinder.
5. Turn the plug with a flat screwdriver and open the door. The cylinder is destroyed - replace it with a new one.

Doing this safely requires safety glasses: spring fragments shoot out of the cylinder like from a slingshot. And there is nothing IT-grade about it - drilling out a lock is field surgery, not precision machining.

Reaming knowledge in a nutshell

To finish, the essence - the things to remember before this operation lands in your process:

• The reaming process improves diameter, form and finish; it does not correct the axis position.
• Typical result: IT7-IT9, with fine reaming IT6; Ra 0.32-1.25 um.
• Too small an allowance is as harmful as too large: the edges rub instead of cutting.
• The parameter rule: low RPM, high feed - the opposite of intuition.
• Feed rate and RPM are calculated as for any tool, but the values come from reamer tables, not drill tables.
• In blind holes the result hinges on flushing the bottom; in deep holes, on guiding the tool.
• Hole finishing always comes after establishing the axis position, never before.
• Accurate holes are a sequence of operations: every IT grade tighter is an extra pass and extra cost.

Reaming is a good example of the broader principle of machining: accuracy is built in stages, and each stage has its own tool, allowance and parameters. Whoever understands that reads a technical drawing like a cost estimate.

Frequently asked questions about reaming

What is reaming in CNC machining? It is a finishing chip-forming operation on a hole: a multi-edge tool removes a 0.05-0.5 mm allowance from the walls of a drilled hole, giving it its final diameter at IT6-IT9 and low surface roughness. In CNC machining it runs as a canned cycle (e.g. G85) right after drilling, in the same setup.

How does CNC reaming work and when does it pay off? CNC reaming means guiding the tool along the hole axis at working feed, with retraction also at feed. It pays off for holes with fit tolerances (H7, H8) up to about 40 mm diameter, especially in series - it is faster than boring and needs no size correction between parts.

What accuracy does fine reaming achieve? Fine reaming routinely delivers IT6-IT8 and surface roughness Ra 0.32-1.25 um. The conditions: a 0.05-0.25 mm allowance on diameter, low cutting speed, generous cooling and rigid, coaxial tool clamping.

How do you drill out a lock cylinder? Centre-punch the plug 2-3 mm above the parting line, drill along the pin line with a 3 mm bit at low RPM with oil, then enlarge the hole with a 4.5-6 mm bit and turn the plug with a screwdriver. It only works on ordinary cylinders - anti-burglary ones contain hardened steel and carbide elements. Drill only your own lock.

Does drilling out a cylinder destroy the lock? Yes, always. Drilling through the pin line irreversibly destroys the mechanism - after opening the door, the cylinder must be replaced. The lock case itself (the bolt mechanism in the door) usually survives, as long as the drill did not go too deep.