Getting reaming right

Author Alan Richter
June 01, 2010 - 11:15am

Appropriate scenarios for applying a reamer when finishing holes.

Appropriate scenarios for applying a reamer when finishing holes. Courtesy of Komet of America.

Courtesy of Komet of America

Cutting rings from Komet have an adjustable diameter range and can be accurately adjusted with special cutting ring holders. This compensates for wear, ensuring the correct adjustment to the exact bore dimension, according to the company.

When machining a hole exactly to size, reaming is often a machinist’s best choice. It typically cannot be used to straighten holes, and can only remove a limited amount of stock, but when done right, reaming can be a fast, highly accurate process. 

Performing reaming correctly, however, requires good preparation. Important factors include leaving the exact amount of stock after drilling; knowing when to ream twice, use a multifunction reamer or use another tool entirely; and specifying the right reamer for the job. Regarding the latter, many different styles of reamers are available—including adjustable, chucking and spiral flute reamers—and in many cases a special is the best tool for the job.

When reaming, preparation of the hole is what’s most important, according to Ryan Bysterbusch, group leader of design engineering for toolmaker Komet of America Inc., Schaumburg, Ill. That’s because a reamer enlarges a drilled hole to size by removing a small amount of stock and does not correct a hole. “The reamer follows the hole,” he said, but noted that a reamer helps to slightly improve straightness if the tool has front-cutting capability.

A selection of chucking reamers from Alvord-Polk. Photo credit: Alvord-Polk

A selection of chucking reamers from Alvord-Polk, including a taper-shank, right-hand, spiral-flute tool. Courtesy of Alvord-Polk.

A selection of chucking reamers, including a titanium nitride-coated, straight-shank, right-hand, spiral-flute reamer. Courtesy of Alvord-Polk.

Courtesy of Alvord-Polk

A selection of chucking reamers from Alvord-Polk, including (above top) a straight-shank, straight-flute reamer; (above middle) a taper-shank, right-hand, spiral-flute tool; and (above bottom) a titanium nitride-coated, straight-shank, right-hand, spiral-flute reamer.

Josh Lynberg, president of tool supplier Monster Tool Co., Vista, Calif., concurred that a “fair-quality” hole is needed before reaming. For example, he noted that when reaming a 0.240 "-dia. hole with a 0.250 " reamer, the hole will not be straightened if it tapers by 0.005 " or more.

If the hole shape or location needs correction, Will Nestor, a Phenix City, Ala.-based application/project sales engineer for toolmaker Mapal Inc., Port Huron, Mich., recommends boring. “But reaming will typically give you a quicker cycle time than boring,” he said, adding that a reamer is more commonly applied to achieve the proper hole size than impart a fine surface finish.

The surface finish obtainable when reaming generally depends on the workpiece material. The range for cast iron is 50 to 80 rms and 30 to 60 rms for steels, and a PCD reamer can impart a finish as fine as 8 rms in aluminum, according to Bysterbusch.

Sometimes a hole is bored prior to reaming, but that’s not mandatory. “Any hole that meets the minimal required amount of stock for the reamed size needs no other preparations before reaming,” Lynberg said. “If the finished hole has an extremely tight tolerance and the machine tool being used to create the hole is not of sufficient accuracy or rigidity, a bored hole helps keep the reamer aligned with the hole axis, assisting the machine tool to keep the hole straight.”

Material Issues

The amount of stock remaining for reaming depends on hole quality and diameter. A rule of thumb is 0.010 " to 0.015 " should remain after drilling for reaming, except for small diameters, such as 1⁄32 ", which should have 0.003 " to 0.006 " of material for reaming, Lynberg noted. “A poorly drilled hole may need a little more material in order for the reamer to ‘clean up’ the hole walls,” he said.

Nestor provided a general DOC range from 0.0039 " to 0.0098 " for Mapal’s guide-padded reamers and up to a 0.0394 " DOC for a brazed-PCD fixed reamer, depending on the workpiece material. “For an aluminum engine component application, we’ve been able to remove up to 1mm per side in the hole,” he said, adding that a larger DOC is possible for a reamer with end-cutting geometry incorporated into the cutting edge.

In addition to aluminum, the stock allowance for magnesium is usually greater than it is for steel, cast iron, titanium and nickel-base superalloys, according to Bysterbusch. If the chip is too thick when reaming the latter materials, too much heat enters the chip, making it ductile and difficult to break, which creates a chip-removal problem. “You’re better off removing as little as you can.”

Others provide more hole-size ranges. Kevin Morrison, chief tooling engineer for Alvord-Polk Inc., indicated that the Millersburg, Pa.-based manufacturer of multiple-flute solid reamers recommends 0.003 " to 0.006 " of stock for reaming holes up to 3⁄32 " in diameter, 0.008 " to 0.010 " for holes larger than 3⁄32 " to ¼ ", 0.012 " to 0.015 " for ¼ " to ½ ", 0.017 " to 0.020 " for ½ " to 1 ", 0.020 " to 0.025 " for 1 " to 2 " and 0.030 " to 0.035 " for holes larger than 2 ". “It’s a sliding scale,” he said. “It doesn’t even work out as a percentage.”

Morrison added that the range is 0.002 " to 0.004 " for a hand reamer. “That’s about all the human body is geared up to do,” he said. “We don’t have the mechanical advantage to take more material out.”

Although some don’t consider material workhardening to be a significant concern when reaming, Nestor noted that it can create challenges. It’s desirable to take a light DOC, for example, when reaming titanium. A light DOC keeps chips thin for ease of evacuation when machining, for example, a small-diameter hole. “Machinability plays a big role in how you ream,” he said.

Sizing the Hole

When too much stock remains for reaming after drilling, end users have the option of reaming twice. Monster Tool’s Lynberg suggests first applying a smaller reamer followed by a reamer of the required size. “Drilling to open up a hole usually causes drill failure due to unequal and uneven stress along the drill’s cutting edge and is not recommended,” he said. Lynberg added that plunge milling is also an option if the proper size endmill is available.

In addition, a step reamer with a roughing and finishing diameter might do the trick. “It depends on the material,” Bysterbusch said. “Once you get into some of the tougher steels, we have to look more in detail at the application.”

Nestor noted that another option is applying a fine boring tool. A fine boring tool has at least three guide pads and is capable of a significantly greater DOC than a reamer. Bore location corrections can also be achieved using a fine boring tool with a cycle time comparable to a guide-padded reamer, he added. 

Part volume also dictates the acceptable solution. “You have to remember the customer always wants to decrease cycle time,” said Donato Pigno, product specialist for Komet. “He’ll typically use a roughing tool and a finishing tool.”

Alvord-Polk’s Morrison suggested that a core drill, which is a cross between a reamer and a drill, can solve the problem when there’s considerably more material to remove than is recommended. A core drill is designed to remove a large amount of material from a hole, but it will not produce a hole by itself. “There are times when a core drill imparts a suitable-enough surface finish that end users use one to finish a hole,” he said.

Tool Considerations

When specifying a reamer, size is the only feature an end user needs to be concerned with unless he’s reaming an unusually deep hole that needs extra tool length, which calls for a special, according to Lynberg. “A properly manufactured reamer will do its job regardless of the material being cut.”

Size is the only feature an end user needs to be concerned about when specifying a reamer. Courtesy of Monster Tool.

Courtesy of Monster Tool

Size is the only feature an end user needs to be concerned about when specifying a reamer, according to Monster Tool.

Although Bysterbusch noted that “full-blown specials” constitute about 40 percent of Komet’s reamer sales, the company’s fixed, monoblock standards are “semispecials.” That’s because standard blanks are ground to size to meet a specific customer’s requirements once the company receives an order. The standard range is from 6mm to 110mm but specials cover a wider spectrum. “We ream everything from 1.5mm to over 300mm,” he said.

Size tolerance plays a role in selecting the style of reamer, according to Mapal’s Nestor. While a fixed tool is appropriate for a larger tolerance range, “any time you’ve got a ±5μm or tighter tolerance on your diameter,” he said, “you want an adjustable reamer.”

Nestor added that chucking reamers can be applied in a drill press, toolroom lathe or even a Bridgeport mill, but guide- padded and other high-performance reamers require a machine with a mechanical feed to provide consistent accuracy. An adequate coolant supply is also required for high-performance reaming. “Typically, soluble oils and semisynthetics work better, but we’ve been successful with synthetic coolant for guide-padded tools,” he said.

Hole interruptions, such as a keyway or cross-hole, also dictate a reaming tool’s requirements. When such a feature is present, Alvord-Polk’s Morrison recommends a spiral-flute reamer so the helix bridges the gap as the reamer rotates and the tool is supported at all times. “If you have a straight flute, every time the tooth comes around it catches and pounds like nobody’s business,” he said.

Regardless of the reaming application, some maintain only an actual reamer will do the job properly. “It is dangerous to say you just want to use a drill with a reaming quality,” said Komet’s Pigno. “You will never get the same result.” CTE

About the Author: Alan Richter is editor of Cutting Tool Engineering, having joined the publication in 2000. Contact him at (847) 714-0175 or


Tool life increased to 50,000 holes when Magna Powertrain USA switched from a carbide reamer to a Dihart cermet-tipped Monomax Solid reamer. Courtesy of Komet of America.

Courtesy of Komet of America

Tool life increased from 1,200 holes to up to 50,000 holes when Magna Powertrain USA switched from a carbide reamer to a Dihart cermet-tipped Monomax Solid reamer from Komet of America when finishing the small hole at the end of 8620 steel actuator levers.

Reaming a 'slick as a whistle' finish 

Reaming holes in 8620 steel with a hardness of 217 HB isn’t necessarily a challenging process—unless you’re doing about half a million of them annually and must achieve tight tolerances, rapid cycle times and low tooling cost per part. Magna Powertrain USA Inc., Muncie, Ind., found itself in that situation when producing actuator levers and having to ream a 0.388 "-dia. by 0.393 "-deep hole on an OKK HP500S horizontal machining center.

David Boxell, a manufacturing engineer for Magna, a producer of components for transfer cases and transmissions, knows the lowest-cost reamer may not be the way to achieve the lowest cost per hole. “I can buy a $35 to $40 reamer off the shelf, but I will only get a few hundred parts, so my cost per unit goes up pretty high,” he said.

Initially, Magna was applying standard carbide-tipped reamers and finishing about 1,200 parts before a tool wore out. The company then switched to custom solid-carbide reamers, with limited success. “They were very expensive and wore down too easily,” Boxell said.

To meet the required finish hole size of 0.3952 " to 0.3948 ", Magna drills a hole from solid and leaves about 0.013 " of stock for reaming. The holes are then reamed oversize so they shrink into the specified dimension when heat treated. No further operations are required after heat treatment.

Previously, Boxell was producing a different product line and during a conversation with another metalcutting professional learned how a Dihart reamer, produced by Komet of America Inc., helped reduce the time to make a part from multiple days to 1 day while holding a 0.0002 " straightness in 4 "-thick holes. Although not entirely convinced, Boxell invited the Komet salesman and the distributor Haggard & Stocking, Indianapolis, to test a Dihart reamer on Magna’s part. “He was right on the money,” Boxell said. “The reamers did exactly what he said they would do.” Magna began using them.

Later, Boxell spoke to Manufacturing Engineer John Hershberger, who was responsible for the actuator levers, and suggested he try the Komet reamer as well. “He loved it and started using it right away,” Boxell said. “Then I inherited the job and now have the whole cell.”

The Dihart 525.91.4030 Monomax Solid cermet-tipped reamer has geometry to push the chips forward. Run at a spindle speed of about 1,800 rpm, the previous reamers took 3 to 4 seconds to finish a hole, whereas cut time for the new tool is 0.14 seconds per bore while running at 4,385 rpm, a 453-sfm cutting speed and a 157-ipm feed rate. The cermet-tipped reamers have through-the-tool coolant, whereas the company applied flood coolant for the carbide ones.

In addition to holding the tight size tolerance, the Monomax reamer imparts a surface finish of 0.6μm Rz when the specification only requires a finish of 1.99μm Rz. “The finish looks ground when we get done with it,” Boxell said. “It’s just slick as a whistle.”

Tool life also significantly improved, going from about 1,200 holes per reamer to 30,000 to 50,000 pieces before losing 4μm to 5μm in size. Boxell noted that he could apply a larger drill and increase reamer life by leaving as little as 0.008 " of stock for reaming, “but I’ve got so many of these other drills in stock that it’s probably not worth buying 200 or 300 drills when the reamer is working so well.”

Although the new custom reamers are priced as a standard and still cost about $400 each, the tooling cost per part went from $0.018 to $0.009. The estimated annual savings is $85,000 not including the cycle time and spindle uptime improvements, according to Boxell. In addition, Magna realizes additional savings by having Komet retip used reamers for about a third of the cost of new. According to Komet, it can retip a tool three or four times. “We bought about 20 of these reamers and have only used four in the last 4 months,” Boxell said, adding that estimated annual tool usage shrunk from 1,000 to 13 tools. “When off-the-shelf tools are done, they’re done.”

—A. Richter


Alvord-Polk Inc.
(800) 441-2751

Komet of America Inc.
(847) 923-8400

Magna Powertrain USA Inc.
(765) 245-9750

Mapal Inc.
(810) 364-8020

Monster Tool Co.

YG-1 Tool Co.
(800) 765-8665

The honed lip on YG-1 Tool’s Dream Drill helps strengthen the edge. Courtesy of YG-1 Tool.
Courtesy of YG-1 Tool

The honed lip on YG-1 Tool’s Dream Drill helps strengthen the edge, the margins help achieve tolerance and surface finish requirements and the helix angle, along with the flute width, enhances chip control and evacuation.

Dreaming of not reaming 

When holemaking, achieving the size and surface finish requirements a reamer provides with just one tool can boost throughput and reduce costs. Although toolmakers have long promoted various drills to eliminate reaming, YG-1 Tool Co., Vernon Hills, Ill., says its Dream Drill also performs center drilling and position boring.


The drill, which is coated with titanium aluminum nitride, can achieve a reamed hole tolerance of M7, according to YG-1 (see Table). Solid-carbide through-coolant drills are available from 0.039 " to 0.787 " and indexable-insert, through-coolant I Dream Drills are available from 0.4724 " to 1.250 ". Drills are also available without coolant holes.

YG-1 offers two designs for machining materials up to 50 HRC: standard for steel, cast iron and similar alloys, and Inox for stainless steel and softer, more ductile alloys. “Small chip curls are always the goal,” said Al Zaitoon, YG-1’s sales and marketing manager.

The toolmaker reports that the Dream Drill’s “S” form web point thinning reduces axial thrust loading and stabilizes the point to produce accurate holes, and the 140° point angle slightly thickens the chip cross section, which helps to break the chips.

Zaitoon noted a Dream Drill’s penetration rate is three to five times faster than a conventional drill, and a 20.00- to 30.00-ipm feed is not uncommon when drilling a 0.250 "-dia. hole in low-alloy steel.

“Generally, the higher the speed, the more ductile the material becomes, therefore reducing the thrust required to drill,” he said, “and the size of the coolant holes are designed to give maximum pressure and volume to reduce heat problems.”

According to Zaitoon, the Dream Drill is suitable for replacing about 50 to 70 percent of reaming applications when drilling from a solid workpiece. Those include applications where the surface finish requirement is specified “as reamed” and the drill can achieve size tolerance. 

—A. Richter

Table: Drill diameter tolerances
Table of drill diameter tolerances.

Related Glossary Terms

  • Brinell hardness number ( HB)

    Brinell hardness number ( HB)

    Number related to the applied load (usually, 500 kgf and 3,000 kgf) and to the surface area of the permanent impression made by a 10mm ball indenter. The Brinell hardness number is a calculated value of the applied load (kgf) divided by the surface area of the indentation (mm2). Therefore, the unit of measure of a Brinell hardness number is kgf/mm2, but it is always omitted.

  • alloys


    Substances having metallic properties and being composed of two or more chemical elements of which at least one is a metal.

  • boring


    Enlarging a hole that already has been drilled or cored. Generally, it is an operation of truing the previously drilled hole with a single-point, lathe-type tool. Boring is essentially internal turning, in that usually a single-point cutting tool forms the internal shape. Some tools are available with two cutting edges to balance cutting forces.

  • center drilling

    center drilling

    Drilling tapered holes for mounting workpiece between centers. Center-drilled holes also serve as starter holes for drilling larger holes in the same location. See centers; drilling.

  • coolant


    Fluid that reduces temperature buildup at the tool/workpiece interface during machining. Normally takes the form of a liquid such as soluble or chemical mixtures (semisynthetic, synthetic) but can be pressurized air or other gas. Because of water’s ability to absorb great quantities of heat, it is widely used as a coolant and vehicle for various cutting compounds, with the water-to-compound ratio varying with the machining task. See cutting fluid; semisynthetic cutting fluid; soluble-oil cutting fluid; synthetic cutting fluid.

  • cutting speed

    cutting speed

    Tangential velocity on the surface of the tool or workpiece at the cutting interface. The formula for cutting speed (sfm) is tool diameter 5 0.26 5 spindle speed (rpm). The formula for feed per tooth (fpt) is table feed (ipm)/number of flutes/spindle speed (rpm). The formula for spindle speed (rpm) is cutting speed (sfm) 5 3.82/tool diameter. The formula for table feed (ipm) is feed per tooth (ftp) 5 number of tool flutes 5 spindle speed (rpm).

  • drilling machine ( drill press)

    drilling machine ( drill press)

    Machine designed to rotate end-cutting tools. Can also be used for reaming, tapping, countersinking, counterboring, spotfacing and boring.

  • endmill


    Milling cutter held by its shank that cuts on its periphery and, if so configured, on its free end. Takes a variety of shapes (single- and double-end, roughing, ballnose and cup-end) and sizes (stub, medium, long and extra-long). Also comes with differing numbers of flutes.

  • feed


    Rate of change of position of the tool as a whole, relative to the workpiece while cutting.

  • finishing tool

    finishing tool

    Tool, belt, wheel or other cutting implement that completes the final, precision machining step/cut on a workpiece. Often takes the form of a grinding, honing, lapping or polishing tool. See roughing cutter.

  • gang cutting ( milling)

    gang cutting ( milling)

    Machining with several cutters mounted on a single arbor, generally for simultaneous cutting.

  • hardness


    Hardness is a measure of the resistance of a material to surface indentation or abrasion. There is no absolute scale for hardness. In order to express hardness quantitatively, each type of test has its own scale, which defines hardness. Indentation hardness obtained through static methods is measured by Brinell, Rockwell, Vickers and Knoop tests. Hardness without indentation is measured by a dynamic method, known as the Scleroscope test.

  • helix angle

    helix angle

    Angle that the tool’s leading edge makes with the plane of its centerline.

  • lathe


    Turning machine capable of sawing, milling, grinding, gear-cutting, drilling, reaming, boring, threading, facing, chamfering, grooving, knurling, spinning, parting, necking, taper-cutting, and cam- and eccentric-cutting, as well as step- and straight-turning. Comes in a variety of forms, ranging from manual to semiautomatic to fully automatic, with major types being engine lathes, turning and contouring lathes, turret lathes and numerical-control lathes. The engine lathe consists of a headstock and spindle, tailstock, bed, carriage (complete with apron) and cross slides. Features include gear- (speed) and feed-selector levers, toolpost, compound rest, lead screw and reversing lead screw, threading dial and rapid-traverse lever. Special lathe types include through-the-spindle, camshaft and crankshaft, brake drum and rotor, spinning and gun-barrel machines. Toolroom and bench lathes are used for precision work; the former for tool-and-die work and similar tasks, the latter for small workpieces (instruments, watches), normally without a power feed. Models are typically designated according to their “swing,” or the largest-diameter workpiece that can be rotated; bed length, or the distance between centers; and horsepower generated. See turning machine.

  • machinability


    The relative ease of machining metals and alloys.

  • machining center

    machining center

    CNC machine tool capable of drilling, reaming, tapping, milling and boring. Normally comes with an automatic toolchanger. See automatic toolchanger.

  • metalcutting ( material cutting)

    metalcutting ( material cutting)

    Any machining process used to part metal or other material or give a workpiece a new configuration. Conventionally applies to machining operations in which a cutting tool mechanically removes material in the form of chips; applies to any process in which metal or material is removed to create new shapes. See metalforming.

  • milling


    Machining operation in which metal or other material is removed by applying power to a rotating cutter. In vertical milling, the cutting tool is mounted vertically on the spindle. In horizontal milling, the cutting tool is mounted horizontally, either directly on the spindle or on an arbor. Horizontal milling is further broken down into conventional milling, where the cutter rotates opposite the direction of feed, or “up” into the workpiece; and climb milling, where the cutter rotates in the direction of feed, or “down” into the workpiece. Milling operations include plane or surface milling, endmilling, facemilling, angle milling, form milling and profiling.

  • milling machine ( mill)

    milling machine ( mill)

    Runs endmills and arbor-mounted milling cutters. Features include a head with a spindle that drives the cutters; a column, knee and table that provide motion in the three Cartesian axes; and a base that supports the components and houses the cutting-fluid pump and reservoir. The work is mounted on the table and fed into the rotating cutter or endmill to accomplish the milling steps; vertical milling machines also feed endmills into the work by means of a spindle-mounted quill. Models range from small manual machines to big bed-type and duplex mills. All take one of three basic forms: vertical, horizontal or convertible horizontal/vertical. Vertical machines may be knee-type (the table is mounted on a knee that can be elevated) or bed-type (the table is securely supported and only moves horizontally). In general, horizontal machines are bigger and more powerful, while vertical machines are lighter but more versatile and easier to set up and operate.

  • plunge milling

    plunge milling

    Highly productive method of metal removal in which an axial machining operation is performed in a single tool sequence. The tool makes a series of overlapping, drill-like plunges to remove part of a cylindrical plug of material one after another. Because of the increased rigidity of a Z-axis move, the tool can cover a large cross-section of material.

  • point angle

    point angle

    Included angle at the point of a twist drill or similar tool; for general-purpose tools, the point angle is typically 118°.

  • polycrystalline diamond ( PCD)

    polycrystalline diamond ( PCD)

    Cutting tool material consisting of natural or synthetic diamond crystals bonded together under high pressure at elevated temperatures. PCD is available as a tip brazed to a carbide insert carrier. Used for machining nonferrous alloys and nonmetallic materials at high cutting speeds.

  • reamer


    Rotating cutting tool used to enlarge a drilled hole to size. Normally removes only a small amount of stock. The workpiece supports the multiple-edge cutting tool. Also for contouring an existing hole.

  • superalloys


    Tough, difficult-to-machine alloys; includes Hastelloy, Inconel and Monel. Many are nickel-base metals.

  • titanium aluminum nitride ( TiAlN)

    titanium aluminum nitride ( TiAlN)

    Often used as a tool coating. AlTiN indicates the aluminum content is greater than the titanium. See coated tools.

  • tolerance


    Minimum and maximum amount a workpiece dimension is allowed to vary from a set standard and still be acceptable.

  • toolroom lathe

    toolroom lathe

    High-precision lathe built to hold tighter tolerances than regular, general-purpose lathes can hold. See lathe; turning machine.

  • web


    On a rotating tool, the portion of the tool body that joins the lands. Web is thicker at the shank end, relative to the point end, providing maximum torsional strength.

  • workhardening


    Tendency of all metals to become harder when they are machined or subjected to other stresses and strains. This trait is particularly pronounced in soft, low-carbon steel or alloys containing nickel and manganese—nonmagnetic stainless steel, high-manganese steel and the superalloys Inconel and Monel.



Alan holds a bachelor’s degree in journalism from Southern Illinois University Carbondale. Including his 20 years at CTE, Alan has more than 30 years of trade journalism experience.