Reamer Guide: Types, Tolerances & How to Choose the Right Reamer

A reamer is the tool that turns a drilled hole into a precision hole. A drilled hole is rough, often slightly oversize, and rarely held to better than ±0.1 mm — fine for a clearance hole on a coach bolt, hopeless for a dowel pin, a fitted bushing or a bearing seat. A reamer takes that drilled hole and finishes it to a tight diameter (typically H7 tolerance, +0.015 mm or so on a 10 mm hole) with a smooth surface finish (1.6 µm Ra is standard, 0.8 µm achievable with carbide and the right setup). The result: a hole that fits its mating part the first time, every time, without filing, lapping or honing.

This guide covers every reamer type encountered in Australian industrial workshops — hand reamers, machine reamers, chucking reamers, adjustable hand reamers, tapered reamers, pipe reamers, Morse taper reamers and shell reamers. The DIN, ISO and ANSI standards that govern them. The pre-ream drill size and stock allowance for any reamer diameter. The speeds and feeds by material. The H7 default tolerance and what dowel pin and bushing fit it produces. And the forum-validated mistakes that cause oversize and undersize holes — and how to fix them.

For Australian workshops, AIMS Industrial stocks the full reamer range — Sutton Tools (Australian-made HSS and cobalt to DIN 206 / DIN 212), Bordo (HSS hand and pilot reamers), and Maxigear adjustable hand reamers across the metric and imperial size ranges. The complete AIMS reamer range is at your call.

What a reamer does — and where it sits in the hole-finishing process

A reamer is a multi-tooth rotary cutting tool that finishes an existing hole to a precise diameter and surface finish. It does not start a hole — that's the drill's job. The reamer follows the drill (or a boring tool) and removes a small amount of material (typically 2–5% of the final diameter) to bring the hole to its final tolerance.

The hole-finishing sequence in a precision-machined part is normally:

1. Centre drill or spot drill to start a precise location.
2. Drill to within 0.1–0.5 mm of the final diameter (size depends on reamer diameter — see the pre-ream drill size table below).
3. Bore the hole if straightness or location accuracy beyond drill capability is required (boring corrects drill drift; reaming alone cannot).
4. Ream to bring the hole to its final diameter (H7 default), with the correct surface finish for the application.
5. Optional: hone or lap for sub-micron finishes (bearing seats, hydraulic cylinders, gauge work).

Reaming is the workhorse precision-finish step in every fitter's, toolmaker's and maintenance machinist's process. It produces dowel pin holes, bearing housing bores, taper pin sockets, bushed pivot points, and the precision pilot holes for press-fit components — the holes that have to be right.

Reamer vs drill bit — the size, finish and accuracy gap

A reamer and a drill bit look superficially similar — both are rotary tools that go in a hole. They are very different cutting tools.

The most important practical takeaway: a reamer cannot fix a crooked or off-centre drilled hole. The reamer follows the existing hole; if the drilled hole walked off, the reamed hole will walk with it. To get a precision-located hole, drill undersize, then bore (or use a precision drilling fixture), then ream. Reaming alone gives you the right diameter and a good surface finish — not the right location.

Hand reamer vs machine reamer vs chucking reamer

This is the most common question on reamers — and the source of more buyer confusion than any other. The three categories overlap. Australian and international catalogues sometimes list chucking reamers and machine reamers as the same thing, sometimes as different products. The differences come down to shank style, lead taper, and intended use:

The terminology nuance: internationally, "machine reamer" and "chucking reamer" are often used interchangeably — both describe a reamer designed for power feed in a chuck or collet. In Australian catalogues (AIMS, Sutton Tools), they are typically listed separately because the shank type matters for tooling: chucking reamers fit a standard drill chuck or ER collet, machine reamers with a Morse taper shank fit the Morse taper socket of a lathe tailstock or drill press spindle directly. If your drill press or lathe has a Morse taper, a Morse taper machine reamer mounts straight in. If you're using a 3-jaw chuck, you want a chucking reamer.

The lead taper difference is the practical reason hand reamers are difficult to use under power: the long lead taper of a hand reamer relies on hand feel for alignment as you turn it. Power-feed it and it digs in unevenly, chatters and produces a poor finish. Machine and chucking reamers have a short chamfer specifically because the machine spindle keeps them aligned — a long lead taper would not improve power-feed alignment and would just waste hole length.

Reamer types — full reference

Beyond the hand/machine/chucking split, reamers are categorised by the hole shape they produce and the application they target. The full type reference for an Australian industrial workshop:

Reamer materials and coatings

Reamer cutting performance depends on the substrate and (sometimes) a surface coating. The choice depends on the workpiece material, production volume, and budget.

For a one-off Australian workshop reamer purchase, HSS in DIN 206 (hand) or DIN 212 (chucking) covers 90% of work. Step up to cobalt for stainless or hard cast iron. Step up to solid carbide only when production volumes justify the cost and the machine has the rigidity to use it.

Flute geometry — straight vs spiral

The flute geometry — straight (axial) vs spiral (helical) — is selected based on the hole geometry, not the material:

• Straight-flute reamer — the default. Lowest cost, cleanest finish on through holes with no interruptions, best for blind holes (chips eject backwards out of the hole, but the straight flute does not pull or push the chip).
• Right-hand spiral reamer (left-hand cut) — pulls chips backward out of the hole. Used on through holes when chip evacuation is critical. NOT for blind holes — chips pile up at the bottom.
• Left-hand spiral reamer (right-hand cut) — pushes chips forward through the hole. Used on through holes where the workpiece is mounted and the chip is to clear the bottom. The geometry that excels at reaming through interrupted holes — cross-holes, keyways, slots — because the spiral keeps the cutting edges in continuous engagement so the reamer does not chatter into the interruption.
• Even-spaced flutes vs unequal spacing — premium reamers use unequal flute spacing (the angles between flutes vary slightly) to break up chatter harmonics. Lower-cost reamers use equal spacing. For precision work, look for unequal-spaced reamers from Sutton, Guhring or premium Bordo.

The Practical Machinist consensus on spiral-flute reamers from years of forum discussion: spiral flutes are essential when reaming through cross-holes or keyways. For straight through holes in regular material, a straight-flute reamer cuts cleaner and lasts longer. Don't pay for a spiral flute unless the geometry calls for it.

Reamer standards — DIN, ISO, ANSI reference

Reamers are made to international standards that specify dimensions, tolerance and shank style. AU industrial drawings reference these standards directly — knowing which is which makes ordering replacements straightforward.

The default tolerance on a reamer-cut hole is H7 — that is, the reamer is ground so it cuts a hole within the H7 ISO 286 tolerance band. For a 10 mm reamer, that gives a hole between 10.000 mm and 10.015 mm. For a 25 mm reamer, between 25.000 mm and 25.021 mm. For specialist applications requiring tighter or looser fits, reamers can be ground to other tolerance classes (H6 for closer, H8 or H9 for slightly looser) — these are special-order items, not stock.

How to use a hand reamer — step by step

Hand reaming is the slow, controlled, precise way to finish a hole. It is the standard technique for fitting work, toolmaking, prototype work, and any single hole that has to be right without setting up a machine.

1. Drill the pre-ream hole undersize. Use the pre-ream drill size table below — typically the reamer diameter minus 0.1–0.5 mm depending on diameter. Too little stock = burnishing and undersize. Too much stock = chatter, oversize, broken reamer.
2. Optional: bore the hole if location accuracy matters. The reamer follows the existing hole — if the drilled hole walked, bore it true before reaming.
3. Mount the reamer in a tap wrench. Use a wrench long enough to give controlled leverage but not so long it lets you over-rotate.
4. Apply cutting fluid generously. Use general cutting oil for steel, kerosene or paraffin for aluminium, soluble coolant for stainless. Lubrication is non-negotiable for hand reaming.
5. Start the reamer square to the work. The long lead taper on a hand reamer self-aligns once started — but only if the first few millimetres are square. Use a square against the shank or visually align with the bore axis.
6. Turn clockwise only — always. Apply steady downward pressure and rotate the wrench clockwise (right-hand cut). Never reverse direction — turning a reamer backward damages the cutting edges immediately.
7. Feed at a steady rate. One full turn = roughly 0.1–0.3 mm of advance for a fine finish. Faster feed = rougher finish; slower feed = burnishing and possible undersize.
8. Reach final depth, then keep turning forward. Continue rotating clockwise as you withdraw the reamer — the cutting edges back-cut on the way out, leaving a clean finish.
9. Clean and inspect. Wipe chips off the reamer flutes, blow out the hole, check the hole with a plug gauge or pin gauge. If the hole is undersize, run the reamer through again with more pressure and oil. If oversize, the reamer was over-fed or has a built-up edge.

Never turn a reamer backwards. This is the cardinal rule of reaming, repeated across every machinist forum from Practical Machinist to Reddit r/Machinists. Reversing the direction during cut OR during extraction dulls the cutting edges immediately and ruins the reamer for any future use. To extract: keep rotating clockwise, slowly withdraw the reamer while it continues to cut on the way out.

How to use a machine or chucking reamer (lathe, mill, drill press)

Machine and chucking reamers are designed for power feed in a machine. The technique is different from hand reaming because the machine controls speed, feed and alignment — but the same fundamentals apply.

1. Drill (and bore if needed) the pre-ream hole. Same stock allowance as hand reaming — refer to the table below.
2. Mount the reamer. Chucking reamer in a 3-jaw chuck or ER collet; Morse taper machine reamer direct in the spindle Morse taper. Use a floating reamer holder if the machine setup may not be perfectly aligned with the existing hole — the float lets the reamer follow the bore.
3. Set the spindle speed. Use 50–67% of the corresponding drilling speed for the same material. See the speeds table below — a 12 mm HSS reamer on mild steel runs at roughly 200–400 RPM (about 60% of the 600 RPM you'd drill at).
4. Set the feed rate. 2–3× the drilling feed rate — counterintuitive, but reamers cut better with a heavier feed. Light feed = burnishing and built-up edge.
5. Apply cutting fluid generously. Flood coolant or generous cutting oil. Reaming generates heat and produces small chips that need flushing.
6. Feed the reamer through the full depth. Smooth, continuous feed — do not pause mid-cut.
7. Stop the spindle, then withdraw under power. The reamer continues to back-cut on the way out, but only if the spindle is running clockwise as you withdraw. Stop the spindle, then withdraw — never reverse the spindle.
8. Inspect. Plug gauge or pin gauge for tight tolerance work; vernier or dial caliper for less critical work.

Floating reamer holders are recommended for chucking reamers when the workpiece location is not exactly aligned with the spindle axis. The holder provides limited radial float (typically 0.5–1.0 mm) so the reamer follows the existing bore rather than fighting it. Without float, a misaligned reamer cuts oversize, bell-mouths the hole entrance, or breaks at the chamfer.

How to use an adjustable hand reamer

Adjustable hand reamers are the universal-finishing tool of the toolmaker, fitter and maintenance machinist. They consist of multiple straight blades that slide in tapered slots in the body — turning end nuts moves the blades up or down the taper, increasing or decreasing the cutting diameter. A typical adjustable reamer covers a 1.5–3 mm size range with a single tool. A full set (Hare & Forbes Precision HSS series TM-A through TM-H, or Bordo / Maxigear equivalents stocked at AIMS) covers approximately 6 mm to 75 mm.

The technique is unforgiving — adjustable reamers are the tool everyone wants until they actually have to use one. The forum-validated procedure:

1. Set the reamer to the smallest diameter that will engage the existing hole. Insert into the hole. Rotate by hand without cutting — confirm the reamer enters cleanly without binding.
2. Adjust upward in small increments. Loosen the upper end nut, tighten the lower end nut a quarter-turn at a time, and re-tighten the upper nut to lock the blades. Do not move the blades by feel without measuring after each adjustment.
3. Measure after every adjustment. Use a vernier caliper across the cutting blades or a micrometer if accessible. Adjustable reamers do not hold a precise diameter against the dial — the blades move slightly under cutting load.
4. Apply cutting oil generously.
5. Cut a small amount, measure the hole, adjust, cut again. Iterate. Do not try to take the full cut in one pass — adjustable blades chatter under heavy load and cut oversize.
6. For final size, use a plug gauge or matching dowel pin to confirm. When the dowel pin is a clean slip fit, you're at size. Stop adjusting.

Adjustable reamer reality check. Forum consensus from r/Machinists, Practical Machinist and the Hobby Machinist: adjustable reamers are slow, finicky, and not suitable for tight-tolerance dowel pin work. They excel at non-standard sizes (a 17.3 mm hole, for example, where a fixed reamer doesn't exist), at field repairs (sloppy keyway in a pulley, worn bushing pocket), and at light cuts in soft materials. For production-grade H7 holes at standard sizes, use a fixed-diameter chucking or hand reamer instead.

Pre-ream drill size and stock allowance

The drilled hole that goes into the reamer must be the right amount undersize. Too little stock and the reamer burnishes rather than cuts (resulting in undersize, glazed finish, premature reamer wear). Too much stock and the reamer chatters, the chip can't escape cleanly, and the hole comes out oversize. The standard rule:

Metric stock allowance per the recognised industry references (Hartner, Helion, M.A. Ford). For imperial stock allowance: under 1/8" → 0.003–0.006"; 1/8 to 1/4" → 0.005–0.012"; 1/4 to 1/2" → 0.008–0.015"; 1/2 to 1" → 0.012–0.025"; 1 to 2" → 0.015–0.040".

Worked example. You need a 10 mm H7 dowel pin hole. The reamer is 10 mm, ground to H7. Pre-ream drill: 10 − 0.3 = 9.7 mm (or 9.8 mm — both work). Drill at 9.7 mm. Optional: bore to 9.85 mm for precision location. Ream with 10 mm H7 chucking reamer. Result: hole between 10.000 and 10.015 mm. A 10 mm m6 dowel pin (10.000 to 10.015 mm) presses in. A 10 mm h6 pin (9.991 to 10.000 mm) is a slip fit.

Rough reaming. A modern Haas or production CNC convention is 3% of reamer diameter as stock allowance — a 10 mm reamer takes 0.3 mm stock per side (matches the metric table above). For rough reaming on production parts where surface finish is less critical, stock can go up to 5% (0.5 mm on a 10 mm hole). For final finish reaming on precision work, stick to 2–3%.

Reaming speeds and feeds by material

Reamers are run at slower speeds than drills — typically 50–67% of drilling speed — and faster feeds. Counterintuitive, but correct: reamers cut better with a heavier feed because the chip thickness has to be sufficient to actually shear material rather than rub it.

Surface speed values per M.A. Ford, Hannibal Carbide and Garr Tool published reaming guides. Convert to RPM using the formula: RPM = (1000 × surface speed in m/min) ÷ (π × diameter in mm). For a 10 mm HSS reamer in mild steel at 20 m/min: RPM = 1000 × 20 ÷ (3.14 × 10) ≈ 640 RPM.

Cutting fluid selection matters for reaming finish. Forum-validated insight from Practical Machinist that contradicts the obvious: cutting oil tends to produce a slightly oversize hole, coolant produces a tighter hole. The mechanism: cutting oil's lubrication reduces friction and chip welding but allows more aggressive cutting; coolant flushes chips faster and cools the reamer, reducing thermal expansion of the cutting edges. For tight tolerance work, use water-soluble coolant. For better finish on tougher materials, use thick cutting oil. For aluminium, use kerosene or specialised aluminium-friendly fluid (never sulphurised cutting oil — it stains aluminium).

Tolerance class, surface finish and dowel pin fits

The default reamer tolerance is H7 — the most common ISO 286 hole tolerance class for fitted components. The H7 tolerance values for typical reamer sizes:

H7 tolerance values per ISO 286-2. Note that the tolerance applies to the hole; the reamer itself is ground undersize so it cuts within the H7 band — different reamer manufacturers grind to different positions within the band.

Surface finish. A correctly used HSS reamer in steel produces 1.6 µm Ra (N7 grade in old notation). With cobalt or carbide and the right speeds and feeds, 0.8 µm Ra (N6) is achievable. For 0.4 µm Ra (N5) or finer, the surface needs honing or lapping after reaming — the reamer alone cannot reliably achieve sub-micron finish.

Dowel pin fits in an H7 reamed hole:

The standard practice: m6 dowel pin in H7 reamed hole = the press-fit pair that locks two parts together permanently. h6 dowel pin in H7 reamed hole = the slip-fit pair that locates two parts but allows removal. Knowing the fit you want determines the pin you order; the H7 reamer is the same in both cases.

Common reaming mistakes and how to fix them

AIMS Industrial reamer range

AIMS stocks the full reamer range for Australian workshops across Sutton Tools (Australian-made, premium HSS and cobalt), Bordo (HSS general-purpose) and Maxigear (adjustable hand reamers). The collections are:

• Reamers — main range — hub for the full AIMS reamer offering. Australian-made Sutton Tools premium reamers alongside Bordo and Maxigear.
• Adjustable Hand Reamers — Sutton Tools, Bordo and Maxigear. Tungsten chrome alloy blades in metric and imperial ranges. The toolmaker's universal-finishing tool.
• Chucking Reamers — for power-feed reaming in lathe, mill or drill press. Sutton R102 series in cobalt steel for stainless and tougher work.
• Taper Pin Reamers — for fitting 1:48 taper pins to lock collars, lever arms and gear hubs. Sutton R105 and Bordo HSS metric.

The Sutton Tools R100 Hand Reamer to DIN 206 is the workshop standard — H7 tolerance, HSS, square drive for tap wrench, in metric sizes from 2 mm up to 25 mm. For shop work where a single hand reamer covers most jobs, this is the call.

For non-standard hole sizes, repair work, or fitting jobs where the hole is between standard reamer sizes, the Maxigear adjustable hand reamer set covers approximately 6 mm to 75 mm with a sequence of 11 reamers — each one adjustable across a 1.5–3 mm range. Replaceable blades extend tool life.

For specific application advice — selecting the right reamer for a particular job, sourcing a hard-to-find size, or matching a reamer to existing equipment — call our team on (02) 9773 0122 or contact AIMS Industrial. We keep reamer-application engineers on hand for exactly this kind of question.

Reamer selection checklist

• Hole final diameter — to the nearest 0.5 mm (or 1/64") for fixed reamers; intermediate sizes call for an adjustable reamer.
• Tolerance class — H7 for standard precision (default); H6 for tighter; H8 or H9 for slightly looser. Specify if non-default.
• Finishing required — 1.6 µm Ra default from HSS; 0.8 µm Ra from cobalt or carbide with right setup; finer requires honing.
• Hand or power feed — hand reamer with square drive for hand tap wrench; chucking reamer with parallel shank for power feed in chuck or collet; Morse taper machine reamer for direct lathe tailstock or mill spindle mount.
• Material to be reamed — HSS for steel, cast iron, soft alloys; cobalt for stainless and hardened steel; carbide for high-volume production.
• Hole geometry — straight flute for through holes and blind holes (blind hole evacuation requires withdrawal-rotation); spiral flute for interrupted holes (across keyways, cross-holes).
• Pre-ream drilling — confirm the pre-ream drill size (refer to the table above) and bore the hole if location accuracy matters.
• Cutting fluid — coolant for tighter tolerance, cutting oil for tougher materials and better surface finish.
• Holder — floating reamer holder for chucking reamers when the workpiece is not perfectly aligned with the spindle.

Frequently Asked Questions

Quick reference answers to the most common questions on reamer types, sizing, speeds and feeds, tolerance and Australian workshop practice.

What is a reamer used for?

A reamer finishes a pre-drilled or bored hole to a precise diameter and surface finish. It is used to bring a hole to its final dimensional tolerance (H7 default — typically +0.015 mm at 10 mm) and to produce the smooth, cylindrical surface needed for fitting dowel pins, bushings, bearings, taper pins or any precision-fit component. The reamer does not start a new hole — it follows an existing hole and refines it.

What's the difference between a hand reamer and a machine reamer?

A hand reamer has a long lead taper (about 25–30 mm) for self-alignment by hand, and a square drive on the shank for use with a tap wrench. It is designed for slow, controlled manual reaming. A machine reamer has a short chamfer (typically 45° × small length) designed to be aligned by the machine spindle, with either a Morse taper shank (DIN 208) for direct mounting in a lathe tailstock or drill press spindle, or a parallel round shank (DIN 212, called a chucking reamer in this case) for mounting in a chuck or collet. Machine reamers run at higher speeds with power feed; hand reamers are turned by hand for fitting work.

Is a chucking reamer the same as a machine reamer?

Internationally, the terms are often used interchangeably — both describe a reamer designed for power feed in a chuck or collet. In Australian catalogues (AIMS Industrial, Sutton Tools), they are typically listed separately to distinguish shank type: a chucking reamer has a parallel round shank for a 3-jaw chuck or ER collet (DIN 212), while a machine reamer typically refers to a Morse taper shank reamer for direct mounting in a lathe tailstock or drill press spindle Morse taper socket (DIN 208). Both have the short chamfer of a power-feed reamer, distinct from the long lead taper of a hand reamer.

What size drill do I use before reaming?

Drill the pre-ream hole 0.1–1.0 mm under the reamer diameter, depending on reamer size. For a 5 mm reamer, drill 4.7–4.8 mm. For a 10 mm reamer, drill 9.7 mm. For a 25 mm reamer, drill 24.5 mm. The metric stock allowance per side is roughly: under 5 mm reamer = 0.1 mm; 5–10 mm = 0.2 mm; 10–20 mm = 0.3 mm; 20–30 mm = 0.4 mm; over 30 mm = 0.5–0.7 mm. The standard production rule is 2–3% of reamer diameter as total stock allowance.

How much stock should I leave for a reamer?

2–3% of the reamer diameter is the standard finish-reaming allowance. For a 10 mm reamer, that's 0.2–0.3 mm per side (0.4–0.6 mm on diameter). For rough reaming where surface finish is less critical, stock can go up to 5%. Too little stock causes burnishing (the reamer rubs rather than cuts, producing an undersize hole and poor finish, and dulling the reamer). Too much stock causes chatter, chip jamming and oversize holes. The 2–3% rule applies to standard HSS and cobalt reamers in steel; carbide reamers can take slightly more stock at higher speeds.

What speed should I run a reamer at?

Reamer speed is roughly 50–67% of the corresponding drilling speed for the same material. For a 10 mm HSS reamer in mild steel, that's about 20 m/min surface speed (about 640 RPM). For aluminium, 60 m/min (about 1,900 RPM). For stainless steel, only 10 m/min with a cobalt reamer (about 320 RPM). Carbide reamers run 2–3× HSS speeds. Feed rate is the counterintuitive part: feed at 2–3× the equivalent drilling feed rate. Light feed causes burnishing; heavier feed allows the reamer to actually cut chips rather than rub.

What tolerance does a reamer hold?

Standard reamers are ground to H7 tolerance — the most common ISO 286 fit class for hole work. For a 10 mm reamer, that's a hole between 10.000 and 10.015 mm. For a 25 mm reamer, between 25.000 and 25.021 mm. Tighter (H6) reamers are special-order; looser (H8, H9) reamers are used where the matching pin or shaft is also at a looser tolerance. The H7 default is a deliberate choice — it matches the m6 dowel pin (interference fit) and the h6 slip-fit dowel that comprise the majority of fitting work.

What surface finish does a reamer give?

A correctly used HSS reamer produces 1.6 µm Ra surface finish (N7 in old notation) — the standard finish for general fitting work, dowel pin holes and bushed bores. Cobalt or carbide reamers running with the correct speeds and feeds can achieve 0.8 µm Ra (N6) — finer than most applications need. For sub-micron finishes (0.4 µm Ra or below) — bearing seats, hydraulic cylinder bores, gauge work — reaming alone is not sufficient; the surface needs honing or lapping after reaming. Common AU shop spec is 1.6 µm Ra unless specified otherwise.

Do I turn a reamer clockwise or anticlockwise?

ALWAYS clockwise — both during cutting AND during extraction. This is the cardinal rule of reaming. Reversing the direction at any point during use damages the cutting edges immediately and ruins the reamer for any future use. To extract: keep rotating clockwise, slowly withdraw the reamer while it continues to back-cut on the way out. The only reamers that turn anti-clockwise are specialty left-hand-cut reamers — these are clearly marked and used in specific applications, not standard shop work.

Why is my reamed hole oversize?

Common causes (in order of likelihood): (1) reamer rigidly held and not aligned with the existing hole — switch to a floating reamer holder; (2) built-up edge on the cutting flutes from chip welding — inspect under magnification, clean with a fine stone, or replace the reamer; (3) too much stock allowance — chips can't clear and jam between flutes, pushing the reamer outward; (4) cutting oil instead of coolant — the reamer expands thermally; (5) excessive RPM with insufficient feed — the reamer rubs and walks. Reduce stock allowance to 2–3%, switch to coolant, increase feed rate, and use a floating holder for chucking reamers.

Why is my reamed hole undersize?

Two main causes: (1) burnishing — the reamer is spinning too fast with too light a feed, so the cutting edges rub rather than shear, work-harden the surface and produce an undersize glazed hole. Reduce RPM and increase feed; (2) the reamer itself is at the bottom of its tolerance band — different manufacturers grind reamers to different positions within H7. Check the actual diameter of the reamer with a micrometer; replace if needed. Less common: too little stock allowance (under 1%), or reaming a hole previously work-hardened by drilling without cutting fluid.

Can you use a reamer in a drill press?

Yes — a chucking reamer mounted in the drill press chuck is the standard low-cost reaming setup for general workshop use. The keys are: (1) match the spindle speed to the reamer speed for the material — drill press lowest speed is often still too fast for a 10 mm reamer in steel, so use the lowest pulley setting; (2) feed steadily and continuously — do not pause mid-cut; (3) apply cutting fluid generously; (4) stop the spindle, then withdraw the reamer — never reverse the chuck. For tight-tolerance work, a floating reamer holder helps the reamer follow the bore rather than fight any spindle-to-bore misalignment.

How do I use an adjustable reamer?

Set the reamer to the smallest diameter that engages the existing hole. Insert and rotate by hand to confirm clean entry. Loosen the upper end nut, tighten the lower end nut a quarter-turn, re-tighten the upper nut to lock the blades. Measure with a vernier across the cutting blades after every adjustment — adjustable reamers do not hold dial-precise size against load. Apply cutting oil, take a small cut, measure the hole, adjust upward, repeat. For final size, confirm with a plug gauge or matching dowel pin — when the pin is a clean slip fit, stop adjusting. Adjustable reamers excel at non-standard sizes and field repairs; for production-grade H7 holes at standard sizes, use a fixed-diameter chucking or hand reamer instead.

What is a chucking reamer used for?

A chucking reamer is the standard machine reamer for power-feed reaming in a lathe, mill or drill press. Its parallel round shank fits a 3-jaw chuck or an ER collet — the most common workshop tool-holding methods. The short chamfer (in contrast to the long lead taper of a hand reamer) is designed for spindle-aligned cutting at production speeds and feeds. Used to produce H7 dowel pin holes, fitted bushings, bearing pilot holes and any precision finishing where the workpiece is mounted in a machine. For Australian workshops, the Sutton Tools R102 chucking reamer to DIN 212 (cobalt steel) is the standard premium choice.

Does Australia use metric or imperial reamers?

Both — metric is the dominant standard for new equipment and modern industrial work, imperial reamers are kept for older equipment and US-spec machinery. Sutton Tools manufactures both metric and imperial ranges in Australia. AIMS Industrial stocks both — metric DIN 206 hand reamers and DIN 212 chucking reamers are the workshop default; imperial reamers (typically to ANSI B94.2) are stocked for fractional-inch holes on older machinery, US-spec equipment and US-imported components. On Australian drawings, metric is the default unless explicitly noted; on US-spec or older drawings, confirm the unit (or look at the dimension format) before ordering.