Reaming: How it Works,Types of Reamers,and Applications

In precision manufacturing, creating a hole is often only the first step. While standard drilling opens up passage in a workpiece, it rarely provides the extreme tight tolerances or smooth surface finishes required for high-precision components like hydraulic valves, bearing seats, or dowel pin alignments.

This is where CNC Reaming comes into play. As a critical secondary machining process, reaming bridges the gap between rough hole-making and ultra-precise hole finishing.

What Is Reaming in CNC Machining?

Reaming is a precision hole-finishing process that uses a multi-fluted cutting tool, the reamer, to remove a thin layer of material from a pre-drilled or bored hole. Its several cutting edges shave the wall evenly to enhance diameter accuracy and surface finish, refining an existing hole into one of the precision holes a bearing, bushing, or dowel pin can actually use. Most of this work runs on CNC machines, though the same reaming process also runs on drill presses and lathes.

A reaming pass typically removes 0.15 mm to 0.35 mm on diameter, which is roughly 0.08 mm to 0.18 mm per side. That controlled material removal is enough to reach micron-level dimensional accuracy, tight roundness, and surface finishes commonly down to Ra 0.8 µm, and as fine as Ra 0.4 µm under ideal conditions.

Reaming vs Drilling vs Boring

All three are hole-making or hole-finishing operations, but they serve different purposes at different stages of the machining process.

Drilling creates the initial hole by plunging a rotating drill bit into solid material. It removes the bulk of the stock quickly, but the resulting hole has limited accuracy, with typical tolerance around ±0.1 mm and a rough finish.

Boring enlarges an existing hole with a single-point tool. Boring tools are used to correct positional error and improve straightness, or to reach hole geometry larger than standard drill sizes. Boring is the right choice when the hole centre must be shifted, not when the goal is simply a fine finish at size.

Reaming uses a multi-fluted rotary cutting tool for light, controlled material removal. Because the reamer follows the pre-existing hole path, that hole must already be reasonably straight and centred before the reaming process begins.

How Does the Reaming Operation Work?

The reaming operation is a finishing step, not a roughing one. The quality of the final hole depends on proper preparation, the right cutting tools, and correct cutting parameters run on a rigid machine tool.

Preparing the Pre-Drilled Hole Size

A reamer follows the pre-existing hole and cannot fix positional error or straightness. The proper hole size before reaming is slightly under the final diameter, so enough material is left for the cutting edges to shear cleanly rather than rub. Getting the proper hole size right is the single biggest factor in a clean result.

Tool-maker guidance is consistent on how much to leave: about 2 to 3 percent of the finished diameter as stock on diameter [1][2]. For a 12 mm hole that works out to roughly 0.24 to 0.36 mm; for very small holes under about 1.5 mm, leave less, around 0.08 to 0.15 mm [2]. Too little stock causes rubbing, a poor finish, and premature tool wear. Too much stock overloads the tool and invites tool breakage.

Tool Selection

Selection depends on the hole type, workpiece material and material hardness, hole size, tolerance, and production volume. High speed steel reamers (HSS) suit general-purpose work in free cutting materials such as mild steel at lower cost. Carbide cutting tools, whether solid carbide or reamers with brazed carbide tips, are the better choice for harder materials, for tight tolerance work, or for long runs where finish must stay stable over thousands of holes.

Flute geometry matters as much as tool material. Straight flutes are the most rigid and work best in short or guided holes. A left hand spiral reamer pushes chips forward and out of through holes, which also limits deflection. A right hand spiral lifts chips back out of blind or deep holes, making it the usual pick for deeper cavities. All of these cutting tools run on CNC machines, drill presses, or lathes, and the right pick is always tied to the specific workpiece material.

Speed and Feed Rates for Reaming

Two rules of thumb drive reaming parameters, and published tool-maker charts agree on both:

• Run slower than drilling. A common cutting speed starting point is 50 to 70 percent of the equivalent drilling speed [3], and some shops go as low as one third to one half of the twist-drill SFM [2]. Running slower speeds protects the finish and helps enhance tool life.
• Feed harder than drilling. Reaming feed is typically 2 to 3 times the drilling feed, because each of the multiple cutting edges takes only a light chip [2][3]. If the feed is too slow, the reamer burnishes instead of cutting. If speed is too high, excessive speed accelerates wear and produces oversized or tapered holes.

Across common materials, reaming speeds generally fall in a 30 to 150 SFM band: soft aluminium alloys tolerate the high end (and beyond with carbide), while tough alloys like titanium sit near 40 SFM [3]. Feed for standard hole diameters commonly runs 0.004 to 0.012 in per revolution [3]. The table below gives conservative HSS starting ranges consolidated from those charts. Add roughly 25 percent to the SFM when the tool is coated [4].

How to Dial In the Numbers on the Machine

Every chart value is a starting point, not a final answer, so start conservative and tune on the machine [4][5]. Bring the SFM up to the low end of the range, then raise the feed in small steps of about 0.001 to 0.0015 in per revolution until finish, size, or chip shape start to degrade, then back off one step [5]. Chip shape is the quickest read on whether the feed is right: continuous, tightly curled chips mean the feed is about right, powdery chips mean it is too low and the reamer is burnishing, and long stringy chips mean it is too high [3]. Steady coolant use throughout the pass keeps built-up edge down and supports a consistent finish across the batch.

The Cutting Process and Material Removal

During the reaming operation the reamer advances through the hole with a continuous feed motion, rotating in a clockwise direction. Its multiple cutting edges each remove a thin slice of stock at the same time, so the radial load stays balanced around the tool. That balanced material removal keeps the hole geometry true and produces superior roundness compared with the one-sided load of single-point boring tools.

Retraction and Coolant

Coolant use runs throughout the pass to lubricate, cool, and flush chips, which also helps enhance tool life. For through holes, the reamer feeds straight through and retracts quickly, and left hand spiral reamers help by pushing chips forward out the exit side, cutting the risk of tool breakage from poor evacuation. For blind holes, the reamer must reverse out at the same feed rate to avoid scoring the finished wall. Chip packing is the main risk in blind or deep holes, and trapped chips will scratch the fine finish unless coolant keeps them flushed.

Types of Reaming Tools and Selection Guide

Choosing the right reamer is half the job. The wrong cutting tools lead to poor finish, short tool life, or scrapped parts. The types below cover the ones you will meet most often.

Chucking Reamers

Chucking reamers are the most common cutting tools for machine reaming, held in a chuck or collet on CNC machines and lathes. They cover the bulk of production hole finishing. Beyond chucking reamers, less common options include shell reamers for large bearing holes, tapered reamers for tapered pins, and combination reamers that carry multiple cutting edges on one body for efficiency.

Hand Reamers

Hand reamers have a long taper lead and a square shank for a tap wrench, and are turned by hand at low speed. They suit fitting work, maintenance, and one-off jobs where a machine setup is not practical. They are not suitable for production.

Machine Reamers

Machine reamers have a shorter chamfer lead and are designed for drill presses, lathes, and CNC machining centers. A machine reamer cuts faster and holds more consistent size than a hand reamer, which is why most CNC reaming on modern CNC machines uses this type.

Straight Flute Reamers

The most common flute style. On straight flute reamers the cutting edges run parallel to the tool axis, which makes the tool rigid and simple to resharpen. Straight flutes work well for through holes in steel, aluminium, and brass, especially where setup rigidity is high and stock is light. They are also preferred in hard materials and guided setups where chip evacuation is less demanding.

Left Hand Spiral Reamers

On a left hand spiral reamer, the flutes wrap around the body in a left-hand helix. That left hand spiral pushes chips ahead of the tool, so it excels in through holes in soft or free cutting materials, and it limits tool deflection while producing a smoother cut with less chatter than straight flutes.

Right Hand Spiral Reamers

A right hand spiral reamer has right-hand cutting edges set in a right-hand helix that lifts chips back toward the shank. That makes it the better choice for blind or deep holes in ductile materials. Good chip control is still needed to avoid packing, but for deeper cavities this geometry clears the finished surface more reliably.

Adjustable Reamers

The cutting diameter can be expanded within a small range by adjusting the blades. These are useful for non-standard hole sizes or for compensating wear. They trade some accuracy for flexibility compared with solid reamers.

Carbide-Tipped Reamers

A steel body with brazed carbide tips. They combine the vibration damping of a steel shank with the wear resistance of carbide cutting edges. A good middle option for medium to high volume production, especially when material hardness is high or the hole diameter is larger. Because carbide is brittle, tool-makers note that below roughly 4 mm (0.156 in) a solid carbide or HSS reamer is usually a better choice than a carbide-tipped one [1].

Solid Carbide Reamers

The whole tool is carbide, giving the best rigidity, wear resistance, and dimensional stability, with optimal performance when setup rigidity is high and tool overhang is minimised. Ideal for high-speed reaming, abrasive materials, and long runs where consistency over thousands of holes matters. The higher cost is offset by longer tool life in volume work.

When Are Reamed Holes Required?

Not every hole needs reaming. Reamed holes should be specified in the design phase under conditions like these:

• Tight dimensional tolerances: when a drawing calls out ISO fit classes such as H6, H7, or H8 that drilling cannot reliably hit.
• High-quality surface finish: when internal surfaces need Ra below 1.6 µm to prevent fluid leakage or reduce friction.
• Alignment and dowel pin placement: press-fit or sliding-fit reamed holes for dowel pins that locate mould bases and machinery.
• Bearing and bushing seats: bores where rotating shafts or bearings need uniform contact pressure.

Advantages and Disadvantages of Reaming

Advantages

• High dimensional accuracy: reaming holds H7 or tighter, a tight tolerance that drilling and boring alone cannot match consistently.
• Superior surface finish: finishes down to Ra 0.4 µm are achievable, often removing the need for honing or grinding.
• Excellent repeatability: the multiple cutting edges deliver consistent size and roundness across large runs with minimal part-to-part variation.
• Fast cycle time: a single pass reaches a tolerance that boring or grinding would take longer to hit.
• Low cost per hole: reamers are inexpensive relative to the holes they produce. With good practice and coolant use, a quality reamer can last tens of thousands of holes, so the cost per finished hole stays low.

Disadvantages

• Cannot create holes: reaming is finishing only. A pre-drilled or pre-bored hole is always required first.
• Cannot correct position: the reamer follows the pre-existing hole path. If the drilled hole is off-centre, the reamed hole will be too.
• Limited stock removal: designed for 0.15 to 0.35 mm on diameter. Beyond that, expect tool damage and poor results.
• Sensitive to setup: poor workholding, low rigidity, excessive runout, or wrong parameters cause chatter, deflection, taper, or oversized holes.
• Faster tool wear in abrasive materials: cast iron, fibreglass, and titanium alloys wear reamers quickly and often justify carbide cutting tools.

Reaming Best Practices for Consistent Hole Quality

Most reaming defects trace back to a handful of avoidable causes. These best practices keep hole quality stable from the first part to the last.

• Control the pre-drilled hole size. Leave the correct stock for the diameter and material. Consistent stock is the biggest driver of consistent finished holes.
• Keep runout under control. Use a high-quality toolholder with less than 0.005 mm runout. Where slight spindle misalignment exists, a floating holder lets the reamer self-align to the hole and reduces the risk of breakage. A floating holder is cheap insurance on older machine tool spindles.
• Feed fast enough to cut. A feed that is too light makes the reamer burnish and glaze the surface instead of shearing a clean chip.
• Flush chips continuously. Keep coolant flowing through the pass and during retraction, and match flute direction to the hole type so chips clear away from the finished wall.
• Maximise rigidity. Minimise tool overhang, support the workpiece, and avoid excessive speed to keep chatter and accelerating wear out of the finish.
• Match the cutting tools to the material. Use carbide or coated reamers for harder materials and abrasive alloys, run slower speeds where heat is a problem, and inspect the cutting edges and chamfer lead for tool wear before it shows up on the part.

Industrial Applications of Reaming

Automotive

Engine blocks, cylinder heads, transmission housings, and brake components all contain reamed holes finished on CNC machines. Valve guide bores, piston pin holes, and connecting rod bores must hold tight fits under high speed and temperature. Reaming keeps these critical bores within H7 across mass production volumes.

Aerospace

Aerospace parts demand extreme precision and leave no room for failure. Reaming is used on turbine shaft bores, landing gear pin holes, hydraulic manifold ports, and structural fastener holes. Titanium and Inconel are common here, and reaming provides the controlled, low-force finishing these harder materials require.

Medical Devices

Surgical instruments, orthopaedic implants, and diagnostic equipment contain precision holes held to strict dimensional and finish standards. Reamed holes in bone screws, implant housings, and fluid delivery components ensure proper fit, smooth flow, and biocompatibility. Finish is especially critical in medical devices, since rough internal surfaces can harbour bacteria or irritate tissue.

Precision Machinery

Mould bases, die sets, linear guide housings, and spindle assemblies rely on reamed holes for accurate alignment. Dowel pin holes in mould plates must be reamed to matching tolerances so the mould halves close in register every time. Spindle bores and bearing seats need consistent roundness and finish to minimise vibration and extend service life.

Common Hole Reaming Problems and How to Avoid Them

Oversized Holes

The most frequent problem. Causes include excessive stock, a worn reamer, too much speed, wrong feed, or tool runout. Check the pre-drilled hole size, verify tool wear on the cutting edges, reduce speed, and use a toolholder with less than 0.005 mm runout.

Poor Surface Finish

Usually a feed that is too low (burnishing instead of cutting), insufficient coolant, or built-up edge on the tool. Increase feed slightly, raise coolant flow, and switch to a coated reamer if built-up edge persists.

Chatter Marks

Visible vibration patterns on the wall, usually from poor rigidity, too much tool overhang, excessive speed, or an unsupported workpiece. Reduce speed, improve workholding, and use a reamer with unequal flute spacing if available, since chatter drives accelerating wear.

Tapered Holes

The diameter varies from entry to exit. This comes from tool deflection under excessive stock, from spindle-to-hole misalignment that distorts hole geometry, or from a worn chamfer lead. Reduce stock, check alignment, and replace worn tools.

Bell-Mouthed Holes

The entry is larger than the rest of the hole, caused by excessive runout, a damaged chamfer lead, or chatter at entry. Ensure a clean chamfer on the pre-drilled hole, minimise runout, and reduce entry feed if needed.

Chips Scratching the Finished Surface

Happens on retraction when chips get trapped between the margins and the wall. Keep coolant flowing during retraction, use spiral-flute reamers for better evacuation, and never retract at rapid traverse in blind or deep holes.

Reaming Case Study

A European client in the automation industry ordered a batch of 304 stainless steel linear guide blocks. Each block had four bore holes designed to accept Ø8.2 mm dowel pins with an H7 tolerance (8.200 to 8.215 mm) and a surface finish requirement of Ra 0.8 µm.

Initial drilling produced Ø8.0 mm holes at roughly Ra 6.3 µm. The drilled holes were round enough, but could not meet the tight tolerance or finish for a press-fit dowel connection. We used a solid carbide straight-flute machine reamer with through-tool coolant, running at a lower cutting speed than drilling with feed suited to the material being reamed. Each hole took about 8 seconds.

The finished holes landed comfortably inside the H7 window with finish to spare.

Frequently Asked Questions About Reaming

Q: What is the difference between reaming and drilling?

A: Drilling creates a hole from solid material and removes most of the stock, but holds only about ±0.1 mm. Reaming uses a rotating cutting tool called a reamer to remove a thin layer from that drilled hole, reaching a tight tolerance and a smooth wall. Drilling makes the hole; the reaming process perfects it.

Q: How much material should be left for reaming?

A: Leave about 2 to 3 percent of the finished diameter on diameter, which is roughly 0.15 to 0.35 mm for most mid-size holes [1][2]. Around 0.2 mm suits most soft materials, and very small holes need less. Too little causes rubbing and poor finish; too much overloads the cutting edges and risks tool breakage.

Q: What tolerance can reaming achieve?

A: Reaming reliably holds H7, and tighter fit classes such as H6 are achievable with rigid setups, carbide tips, and controlled parameters. Surface finish typically reaches Ra 0.8 µm, and Ra 0.4 µm under ideal conditions.

Q: What speed and feed should you use for reaming?

A: Start at about 50 to 70 percent of the drilling speed and 2 to 3 times the drilling feed [2][3]. Slower speeds with a higher feed help the cutting edges shear cleanly instead of burnishing. Exact figures depend on material, tool, and your CNC machines, so treat published charts as starting points to verify.

Q: When should you use a left hand vs a right hand spiral reamer?

A: Use a left hand spiral for through holes, since it pushes chips forward and out the exit side. Use a right hand spiral reamer for blind or deep holes, since its right-hand cutting edges lift chips back toward the shank and away from the finished bottom.

Sources and Further Reading

1. Super Tool, Inc. “Reaming Speeds and Feeds.” https://www.supertoolinc.com/blog/reaming-speeds-and-feeds/
2. CNCCookbook. “Easy Guide to Reamer Speeds and Feeds, Sizes, Types, and Tips.” https://www.cnccookbook.com/easy-guide-to-reamer-speeds-and-feeds-sizes-types-and-tips/
3. “Reamer Cutting Speed: Optimal Parameters for Precision Machining.” https://www.magotan-tools.com/news/industry-news/reamer-cutting-speed-optimal-parameters-for-precision-machining.html
4. Fullerton Tool Co. “Speeds and Feeds (Reaming).” https://fullertontool.com/media/Fullerton-1415-Speeds-Feeds.pdf
5. Hannibal Carbide Tool. “Reamer Guide: Basic Technical Information for Reamers.” https://www.hannibalcarbide.com/wp-content/uploads/2024/02/cost-effective-reaming-guide.pdf