Reaming FAQ

A reamer is a precision cutting tool used to slightly enlarge and finish a previously drilled or bored hole. Its purpose is to improve hole size accuracy, surface finish, roundness, and consistency.

The right reamer depends on the material being machined, whether the hole is blind or through, the required tolerance, the desired finish, and the rigidity of the setup. Tough or abrasive materials often require stronger substrates, carbide or carbide-tipped tools, and more wear-resistant geometries. Check out our Reaming Guide for deeper insight into factors to consider when choosing the right reamer for you.

Hard, tough, abrasive, sticky, or work-hardening materials usually require more specialized reamers. Stainless steel, titanium, and similar alloys often need stronger edge support, optimized clearances, and wear-resistant materials. Softer or free-cutting materials like aluminum and brass may need flute geometry that prevents chip welding or overfeeding.

Each flute style affects chip flow and cutting behavior differently:

• Left-hand spiral reamers push chips forward and are often best for through holes.
• Right-hand spiral reamers pull chips back out of the hole and are often preferred for blind holes.
• Straight flute reamers offer high stiffness and are commonly used in short holes, hard materials, interrupted holes, and guided or manual work.

Use a left-hand spiral reamer for through holes, especially where you want chips pushed ahead of the tool and out the far side. They are especially helpful in free-machining materials and in interrupted holes or cross-hole features where smoother re-engagement is important.

Use a right-hand spiral reamer when reaming blind holes or deep cavities where chips need to be lifted out of the hole. They are often useful in ductile or stringy materials, but they must be used with good chip evacuation and feed control to avoid self-feeding too aggressively.

Straight flute reamers are a good choice for short holes, rigid setups, hand reaming, guided reaming, interrupted holes, and harder materials where stiffness and alignment matter more than active chip lifting.

Hand of cut describes the cutting rotation direction. Hand of spiral describes the direction the flutes twist. These are not the same thing, and both matter when selecting the right reamer for chip control and cutting behavior.

No. A smooth finish does not guarantee size accuracy, roundness, straightness, or concentricity. A hole can look good visually and still be tapered, bell-mouthed, or out of tolerance.

Hole accuracy is affected by tool geometry, rigidity, spindle runout, holder concentricity, machine condition, alignment, stock allowance, feed rate, coolant, and overall setup stability.

If the cutting edges are not concentric with the shank and tool body, the reamer can load unevenly during cutting. This can cause premature wear, inconsistent hole geometry, poor finish, and reduced repeatability.

A common starting point is to run reaming at about two-thirds of the drilling speed for the same material. In many cases, especially for finish and close-tolerance work, slower speeds may be necessary to prevent chatter and protect tool life.

Reaming feeds are often higher than drilling feeds. A common starting range is about 0.0015" to 0.004" per revolution, depending on the material, diameter, setup, and finish requirement. Too light a feed can cause rubbing and work hardening; too heavy a feed can reduce accuracy and finish quality.

If the feed is too low, the reamer may rub or burnish instead of cutting. That can glaze the hole, work-harden the material, increase chatter, and accelerate tool wear.

Excessive feed can overload the reamer, increase deflection, worsen finish, reduce dimensional accuracy, and in some cases chip or break the cutting edges.

Blind holes generally require more conservative settings. Chips cannot exit the far end, so they accumulate and are more likely to be recut or packed, increasing heat and cutting pressure. Reducing speed by 10-20% and using through-tool or high-pressure coolant helps flush chips during the cut. Through holes allow more aggressive parameters since chips clear naturally, but feed should still be consistent to avoid chatter or witness marks on withdrawal.

Common symptoms include:

• Chatter or vibration — often excessive speed or insufficient feed. Reduce speed and increase feed slightly.
• Poor finish or torn material — usually too little feed, causing rubbing instead of cutting.
• Oversize holes — can result from chatter or excessive speed.
• Rapid tool wear — may indicate too much speed generating heat, or too heavy a feed overloading the cutting edges.
• Built-up edge on the flutes — common when speed is too high or feed too light, especially in aluminum and stainless.

Adjust one variable at a time — speed first, then feed — so the effect of each change can be isolated.

Stainless steel (like 304 or 316) and Inconel tend to work-harden quickly. To succeed:

• Use Cobalt (M42) or Carbide tools for better heat resistance.
• Select an AlTiN coating to provide a thermal barrier.
• Ensure a positive, constant feed. If the tool dwells or rubs, the material will harden, making further reaming nearly impossible.

Aluminum is soft and "gummy," which often leads to built-up edge (BUE). For the best results:

• Use Spiral Flute reamers to clear chips efficiently and prevent "bird-nesting."
• Use a Bright (Uncoated) tool with highly polished flutes or a ZrN (Zirconium Nitride) coating.
• High-pressure coolant or mist is essential to keep the flutes clear and the material cool.

Cast iron is highly abrasive but often produces small, crumbly chips rather than long strings. Straight flute reamers are often the standard choice here due to their rigidity. Because cast iron is abrasive, TiCN coating or Carbide-tipped tools will significantly extend tool life compared to standard HSS.

Plastics have a tendency to "close up" after the tool is removed due to heat expansion. You may need to use a reamer that is slightly oversize to account for this recovery. Sharp cutting edges are mandatory; a dull tool will tear the fibers in composites (like G10) rather than shearing them.

Work-hardening occurs when the heat and pressure of the machining process change the molecular structure of the material, making it harder than the cutting tool. To avoid this, never let a reamer "dwell" in the hole. Use sharp tools, proper coolant, and a heavy enough feed rate to ensure the tool is always cutting fresh material.

Hardened steel above roughly 45 HRC requires carbide reamers — HSS grades lack sufficient hardness to cut effectively at that range. Use a high-heat-resistant coating such as AlTiN or AlCrN, keep speeds conservative, and maintain a steady feed to avoid dwelling. Setup rigidity is critical; carbide is brittle enough that chatter can cause chipping or fracture. Flood or through-tool coolant helps manage heat, and pre-finishing the hole as accurately as possible before reaming reduces load on the tool.

Sharp cutting edges are essential — dull tools drag and smear soft metals rather than cutting cleanly. A CrN or ZrN coating, or an uncoated bright-finish reamer with polished flutes, reduces friction and material adhesion; avoid TiN and AlTiN. Straight flute reamers work well for most brass. Use soluble oil or semi-synthetic coolant for lubrication, and avoid excessive feed, which can cause material to flow ahead of the edge rather than shear cleanly. Copper is stickier than brass and may need extra attention to edge sharpness and coolant flow.

High-Speed Steel (HSS) and carbide represent two different tool substrate families, each with distinct trade-offs. HSS reamers are tougher, easier to resharpen, and more forgiving in setups with vibration or minor misalignment. Carbide reamers are significantly harder and more wear-resistant, holding their edge longer in abrasive or high-production applications — but they are more brittle and more sensitive to interrupted cuts, misalignment, and chatter. The right choice depends on the material being machined, the required tolerance, and the rigidity of your setup.

These four properties define how a tool substrate performs in the cut and how it can be maintained:

• Wear resistance — how well the cutting edge holds up against abrasion over time. Higher wear resistance means longer tool life, especially in abrasive or hard materials.
• Toughness — the material's ability to absorb impact and resist chipping or fracture. This matters most in interrupted cuts, cross-holes, or setups with vibration or minor misalignment.
• Red hardness — the ability to retain hardness at elevated temperatures. A tool with high red hardness can run at higher speeds or in hotter conditions without the cutting edge softening and losing its shape.
• Ease of grinding — how readily the tool can be resharpened. Tools that are easier to grind require less wheel wear and simpler technique to restore a good cutting edge. Carbide is the most difficult to regrind of any common reamer substrate.

M2 is the most widely used general-purpose HSS grade. It offers a well-rounded combination of wear resistance, toughness, red hardness, and ease of regrinding, making it a reliable and cost-effective choice for most everyday machining applications — mild steel, aluminum, brass, and plastics in standard production environments. It is not the top performer in any single category, but its balance across all four makes it the default starting point for many shops. Where high heat, aggressive feeds, or abrasive materials are a factor, a higher-grade HSS or carbide is usually the better choice.

M42 is a cobalt-bearing HSS grade with exceptional red hardness — among the highest of any standard HSS. The added cobalt allows it to retain cutting edge hardness at elevated temperatures, making it well-suited for stainless steel, titanium, and heat-resistant superalloys where work-hardening and heat generation are significant concerns. It offers better wear resistance than M2 as well, though its toughness is somewhat lower. The main trade-off is that M42 is harder to regrind than standard HSS grades, so proper grinding equipment and technique are important to maintain edge geometry when resharpening.

Powder metal HSS grades — including PM M4, PM T15, PM M48, and PM A11 — are manufactured by sintering fine metal powders rather than conventional casting and rolling. This process produces a far more uniform distribution of carbide particles throughout the steel matrix, which is what drives their performance advantage. Conventional manufacturing creates carbide segregation and uneven grain structure that limits how much alloying is practical. PM processing removes that limitation, allowing much higher alloy content without sacrificing toughness. The result is significantly better wear resistance and, in grades like PM M4, substantially higher toughness than a conventionally made tool of the same designation. PM grades are the preferred choice for demanding applications where both edge life and resistance to chipping are required.

PM M4 is widely regarded as the best-balanced HSS grade for applications that demand both long edge life and resistance to chipping or fracture. Its powder metal construction gives it exceptional toughness alongside high wear resistance — a combination that conventional HSS grades cannot achieve at the same level. It is an excellent choice when the application involves abrasive materials, interrupted cuts, or setups that are not perfectly rigid. For applications where the cut is smooth and continuous and maximum wear resistance is the priority, PM A11 or PM M48 push the wear resistance higher, though with somewhat less toughness than PM M4.

The cobalt percentage in a carbide grade refers to how much cobalt binder is used to hold the tungsten carbide particles together, and it directly controls the trade-off between hardness and toughness. Lower cobalt content means a harder, more wear-resistant grade — but also a more brittle one. Higher cobalt content adds toughness at a slight cost to hardness and wear resistance.

• C2 Carbide at 6% cobalt is the hardest option available, with maximum wear resistance and red hardness. It is best suited for rigid setups, smooth non-interrupted cuts, and high-production work in abrasive materials. It has the lowest toughness and is the most difficult to regrind of any common grade.
• C2 Carbide at 10% cobalt gives up a small amount of hardness in exchange for meaningfully better toughness. It retains near-maximum wear resistance and red hardness, making it the safer carbide choice when some vibration, interrupted cutting, or setup variability is present.

For most reaming applications, the 10% grade is the more practical starting point unless the setup is known to be highly rigid and the cut is continuous.

Carbide's extreme hardness — which is what makes it so wear-resistant in the cut — also makes it very resistant to the grinding process itself. Standard aluminum oxide or silicon carbide wheels used for HSS have almost no effect on carbide. Diamond grinding wheels are required, and the process is slower, more expensive, and demands greater skill and precision to restore correct geometry without introducing micro-cracks or heat damage to the cutting edge. For most shops, carbide reamers are either replaced outright or sent to a specialist regrind service rather than resharpened in-house. This is a meaningful cost consideration, particularly in lower-volume applications where a more easily reground HSS grade may offer better overall economics.

Not always. Carbide's advantages in wear resistance and red hardness are most valuable in high-volume production, abrasive materials, and high-speed applications where edge life directly affects output and cost. However, carbide's relatively low toughness makes it vulnerable in conditions where a tougher HSS grade would perform reliably: setups with vibration or chatter, interrupted holes, cross-holes, slight misalignment, or machines with worn spindle bearings. In those situations, a tough PM HSS grade will often outlast carbide — not because it holds an edge longer under ideal conditions, but because it survives conditions that would chip or fracture a carbide tool. Setup quality and rigidity are often the deciding factor when choosing between carbide and high-performance HSS.

For maximum wear resistance and temperature resistance in hard, abrasive, or high-speed applications, C2 carbide at 6% cobalt is the top performer — provided the setup is rigid, the cut is continuous, and the machine is in good condition. If some toughness is needed alongside abrasion resistance, C2 carbide at 10% cobalt or a top-tier PM HSS grade like PM M48 or PM A11 offer strong wear performance with more tolerance for real-world conditions. For work-hardening alloys such as stainless steel and titanium specifically, high red hardness is the critical property — M42, PM T15, or PM M48 are often preferred because they resist softening at the elevated temperatures those materials generate during cutting.

A common rule of thumb is about 3% of the hole diameter, though actual stock allowance depends on hole size and application. In many finishing operations, a typical allowance is about 0.004" to 0.012" on diameter.

If there is too little stock, the reamer may not cut cleanly. Instead, it may burnish the hole, causing poor finish, work hardening, and inaccurate results.

Too much stock can overload the reamer, increase cutting pressure, cause deflection, reduce hole accuracy, and shorten tool life.

Generally, yes. Through holes are usually easier because chips can exit the far side. Blind holes are more difficult because chips can pack at the bottom and damage the tool or hole surface.

Use a reamer suited for blind-hole chip evacuation, control the depth carefully, avoid bottoming out the tool, and provide adequate coolant or flushing to keep chips from packing at the bottom.

No. Reamers should not be rotated in reverse to exit the hole because doing so dulls the cutting edges. Keep the reamer rotating in the cutting direction during withdrawal whenever possible.

A feed-in, feed-out cycle such as G85 is often preferred because it helps produce better bore finish and minimizes witness marks. Rapid-out or spindle-stop retract cycles can leave marks on the bore wall.

No. Pecking interrupts the cut and can damage finish, worsen alignment, and increase the chance of marks or chatter. Reaming should generally be done in one smooth, continuous feed.

Misalignment between the spindle, holder, bushing, and hole can cause bell-mouthing, taper, oversize holes, reduced straightness, poor finish, and shorter tool life.

Floating holders help the reamer self-align during cutting. They are useful when machine condition, fixturing, or setup may create angular or parallel misalignment. They can reduce bell-mouthing, uneven loading, and premature wear.

No. They help compensate for some misalignment, but they are not a cure-all. Machine wear, poor holder condition, weak fixturing, and excessive setup error can still create poor results.

A piloted reamer includes a pilot section that works with bushings or guide features to help maintain alignment. These are especially useful for long holes, closely controlled locations, and line reaming applications.

Bushings guide the reamer and improve alignment, which helps reduce taper, tool wear, and hole location error. Proper fit and lubrication are important to prevent binding or damage.

Not usually with plain reaming alone. When concentricity across multiple holes matters, line reaming with guided tooling and progressively sized holes is generally required.

Chatter is often caused by excessive speed, insufficient feed, weak fixturing, too much overhang, loose holders, poor machine rigidity, misalignment, or unsuitable flute design.

Lower the speed, maintain a steady feed, improve setup rigidity, reduce overhang, correct alignment issues, and use the appropriate reamer geometry for the material and hole type.

In reaming, coolant is used primarily to improve finish and help flush chips, not just to reduce heat. Good lubrication and chip evacuation are essential for consistent results and long tool life.

Common causes include lack of rigidity, excessive cutting forces, poor chip evacuation, vibration, chatter, misalignment, inconsistent feed, tool overload, and improper sharpening or handling.

Less obvious causes include dirt or burrs in holders, lack of lubrication between guide bushings and reamers, bent shanks, worn spindle bearings, poor sharpening practices, and built-up material on the cutting edges.

Reamers should be stored separately in racks or boxes so the cutting edges do not contact each other. A light protective oil coating helps prevent rust and edge damage during storage.

Yes. Even a small nick, burr, or rust pit on a flute can reduce finish quality, affect hole size, and shorten tool life.

Reamers should be reground before they become severely dull. Waiting too long can reduce performance, harm hole quality, and make it harder to restore proper geometry.

Usually the chamfer is resharpened, since tool diameter is often critical and must be preserved.

Hand sharpening can create uneven cutting edges or flute geometry, which can lead to oversize holes, poor finish, chatter, and inconsistent performance.

Rigidity is the tool and setup’s resistance to deflection under load. High rigidity improves dimensional accuracy, finish, repeatability, and tool life. Low rigidity increases vibration, wear, and scrap risk.

If chips are trapped, packed, or recut, they can damage the cutting edges, scratch the hole wall, increase heat, and cause premature failure.

Tolerance is the allowable variation from a specified dimension. It defines the acceptable size range a part feature can have and still function correctly.

Tolerance matters because it ensures proper fit, interchangeability, reliability, and performance. If holes or other features fall outside tolerance, components may not assemble properly or may fail in service.

An oversized hole may create a loose fit, vibration, or reduced holding strength. An undersized hole may prevent assembly, require rework, or damage mating components.

Common types include:

• Limit tolerances – maximum and minimum allowable size
• Unilateral tolerances – variation allowed in only one direction
• Bilateral tolerances – variation allowed above and below nominal size

A diameter of 0.2756" with a tolerance of ±0.0002" means the acceptable range is 0.2754" to 0.2758".

In high-performance industries, even small dimensional errors can affect fit, structural integrity, fatigue life, safety, and inspection compliance. Tight tolerance control helps prevent failures, rework, and costly rejects.

Typical straight reamer tolerances are:

• Up to 1/2": +0.0002" / -0
• Over 1/2" to 1 1/2": +0.0003" / -0
• Over 1 1/2": +0.0004" / -0

Yes. Designing parts so the reamer can pass through the hole, minimizing difficult blind-hole conditions, allowing clean entry, and supporting proper alignment can all improve hole quality and reduce tool wear.

Check the full process, not just the tool. Look at stock allowance, feed, speed, alignment, holder condition, spindle runout, rigidity, coolant, chip evacuation, and hole type. Fast wear is often caused by several small issues happening at once.

Use the correct reamer for the material and hole type, leave proper stock, maintain alignment, choose steady feeds and conservative speeds, avoid chatter, ensure good coolant flow, and regrind tools before they become badly worn.