Kennametal Machining Guide: Reaming Tool Basics

But what is reaming, anyway? Simply put, a reamer is a multi-tooth, rotary cutting tool that removes relatively small amounts of material along its leading edges as it passes. It is considered a finishing tool, and requires a pre-drilled hole of a specific diameter to function properly. Straight-flute and helical designs are available, as are so-called left-hand and right-hand versions of the latter (more on this shortly).

Machinists face a bewildering number of choices when selecting a reamer. Shell, Rose, Hand, Taper, Structural…it’s an extensive list. For most applications, however, CNC and manual machinists will use either a Machine reamer or a Chucking reamer, in that order. Expandable reamers are another option, especially for larger holes (say anything above 3/4″ or so) or where it’s difficult to achieve the proper hole size. And as you’ll see, modular reaming systems with replaceable heads have become an attractive option over recent years.

Machinists must also decide whether to use carbide or high-speed steel (HSS) reamers. The latter is perfectly fine for softer materials such as aluminum and plastic, and in limited production runs where tool life is less of a concern. For all else, carbide-tipped, modular, or solid carbide tools are preferred. Some cutting tool providers (Kennametal is one) also offer reamers with brazed polycrystalline diamond (PCD) tips; though more expensive than the alternatives, these high-performance tools are ideal for higher volume work in abrasive materials like high silicon aluminum, carbon fiber composites, and certain glass-filled polymers.

Although a properly applied reamer can provide excellent hole quantity and accuracy within a few ten-thousandths of an inch—and do so very quickly—some caveats exist. Perhaps the most notable of these is the well-known adage that “reamers follow the hole.” This means that any runout or drift during the drilling operation will remain after reaming. It’s for this reason that properly preparing the hole beforehand is crucial.

1. Start by spot-drilling the workpiece face. This will keep the drill from wobbling as it enters the workpiece and help to increase hole straightness. Use an NC spotting drill for this operation rather than a center drill, which is designed to create grinding centers in shafts (not starter holes). If using a solid carbide drill, however, this spotting step can usually be eliminated. It’s also a good idea to run the spot drill deep enough to chamfer the hole slightly chamfer, which will help guide the reamer as it begins cutting—for example, a 0.25″ finished hole size should be chamfered to 0.27″ diameter, give or take.
2. Drill the hole to the recommended size for reaming. Follow the manufacturer’s guidelines here, but a good rule of thumb is to drill the hole approximately 3% smaller than the finished hole. For instance, a 1/8″ diameter reamed hole should be drilled with a #31 drill bit (0.12″), whereas a 3/4″ reamer would require either a 47/64″ (0.734″) or 18.5 mm (0.728″) starter hole. Leaving too much material behind will lead to chip packing and possible tool breakage, while too little causes the reamer to rub rather than cut, resulting in poor tool life and surface quality.
3. Ream the hole. Here again, it’s important to follow the cutting tool manufacturer’s feed and speed recommendations, but some suggest a cutting speed of one-half to two-thirds that of drilling and a feedrate two to three times higher. That said, the machinist must consider several variables, including the cutting tool material (HSS runs at speeds roughly one-fourth that of carbide), the reamer’s flute count (more cutting edges mean a faster overall feedrate), hole depth and diameter, workpiece material, machine tool and setup rigidity, and whether coolant is being used.

In a perfect world, the result is a straight, round hole with a fine surface finish and predictable size control. Unfortunately, we don’t live in this world, and as with any machining operation, numerous factors can hamper success. As noted earlier, reamers tend to “follow the hole,” and if the drill walks, so will the reamer. Here’s another instance where solid carbide reamers have an advantage, as they are less prone to deflection, but to mitigate hole walk as much as possible, follow the spot drilling and chamfering advice already given; if that’s not sufficient, some machinists will use a boring bar or end mill to “true the hole” a diameter or two deep (and slightly undersize) before reaming.

Opinions vary on this next part. Some will argue that reamers should made to run perfectly true in the toolholder using a dial indicator and a few gentle nudges with a plastic mallet or piece of brass, which is good advice for any rotary tool. Others suggest that the reamer’s going to follow the hole regardless, so a floating toolholder should be used, which allows the reamer to “go its own way.” Kennametal’s recommendation is to use a floating holder where misalignment is present, but to select a high-quality collet chuck, shrink-fit, or hydraulic toolholder for minimal runout in all other cases. Don’t use a drill chuck or side-lock holder.

Opinions also vary when it comes to cutting fluid, but whether your shop uses neat oil, synthetic, or water-soluble emulsion, it should be clean and well-maintained. For those with through-the-tool capabilities, by all means use it, even though this might mean upgrading to a solid carbide or modular-style reamer. That statement holds true for high-pressure coolant (HPC) as well, which can spell the difference between success and failure in many machining applications, reaming included.

There’s also the programming to consider. CNC machinists using FANUC or compatible controls (which is most of them) have several options. For CNC lathes, a simple G01 command is all that’s needed, feeding into the workpiece at the recommended rate and then retracting with a G00 rapid traverse command or an accelerated feedrate. CNC machining centers can use this same approach, although the G85 or G86 boring cycles are another option. The latter of these stops the spindle when the tool reaches full depth and then rapids out, while G85 feeds in and out at the same feedrate. Experiment with each and see what provides the best results for your application, but in no case should you peck the reamer as you would a non-coolant fed drill.

In no particular order, here are a few other factors to think about when preparing for or troubleshooting your next reaming operation:

• Reamers with a left-hand helix tend to push the chips forward during machining. These should be used on through-holes or where generous chip space exists. For all else, select a tool with straight flutes (for short chipping materials like brass and cast iron) or a right-hand helix (for stringy materials) to avoid chip packing in the bottom of the hole.
• More flutes mean a faster feedrate can be used but with less room for chips. If packing is a concern, select a reamer with a lower flute count. Also, reamers tend to cut slightly larger than nominal, so it’s a good idea to choose one at the bottom of the hole’s tolerance band. If available, adjustable reamers with brazed carbide tips are also a great choice (albeit with a higher price tag).
• Speaking of carbide, if your shop is still using the HSS chucking reamers that date back to the Brown and Sharpe screw machine days, consider upgrading to a solid carbide or even a modular reamer (check out Kennametal’s RHM-E series as an example). Both boast advanced coatings and micrograin carbide for maximum tool life and increased productivity.

There’s more. Modifying the reamer’s chamfer amount and angle can help address challenging hole conditions and materials, although this must be done in a precise manner using specialized tool grinding equipment. Similarly, it’s important to inspect reamers before use. Check for chipping and wear, and replace the tool sooner rather than later. And if you run into trouble, don’t hesitate to reach out for help. Kennametal has dozens of metal removal experts available, ready to lend a hand with this and other machining applications.