High Expectations

Expect quite a bit from the reaming process, particularly those of us in the aerospace industry. In my experience with the manufacture of aircraft components, where reaming was the most cost-effective solution, I’ve seen diametrical tolerances as small as 0.0002" for holes. Moreover, the callouts for surface finishes often run as fine as 16 Ra (about 0.3µm).

An engineering society once published a graph that suggested a diametrical tolerance of 0.0005" was located at the “ragged edge” of reaming’s process capability. My experience, and a fair amount of hard data, indicates that this is usually true. This “truth” creates some genuine challenges.

Consider that the diametrical tolerance for a reamer is generally 0.0002". When we factor in straightness, runout and gaging error, and consider the setup and application variables, it’s easy to understand why the machinist or manufacturing engineer can soon find a reaming operation entirely out of tolerance.

In the following we’ll look at some of the factors that affect the quality of reamed holes, concentrating on tools ground from a solid that have diameters of 0.080" to 0.500".

Tool Mounting, Feed, Machines
Tool mounting is a big consideration when reaming. Runout must be controlled. Conventional wisdom tells us that the way around runout is to use a floating holder. It lets the reamer “float” in the radial, axial or angular direction. This is a legitimate solution in many applications, such as when the drilling and reaming of the hole are not done in the same fixturing.

But in cases where drilling and reaming are performed in the same setup, centerline mismatch of the drilled hole to the reamer is not an issue. Therefore, any degree of float—including that from a floating holder—will tend to be counterproductive. However, when using a solid mount, it is critical to control the tool’s radial runout to compensate for inaccuracies in the holder, collet or reamer.

As for feed rates, there is no hard-and-fast rule. But a 0.003 to 0.012 ipr feed is generally needed to achieve optimum results. The key is to use a feed rate low enough to avoid a rough finish and the oversize condition caused by overloading the tool, while allowing a reasonably sized chip to form where the cutting chamfer meets the flute or rake face of the reamer.

Modern practice dictates the use of a rigid, accurate machining center when striving to hold the tight tolerances of a reaming process. And using a CNC that allows infeed rates to be programmed in inches per revolution—rather than inches per minute—will save a calculation when it comes to establishing and controlling feed rates.

A lot of people in the metalworking industry cut their teeth by “jumping Bridgeports.” This ubiquitous manual mill, which remains a mainstay of many small shops, is a viable machine for reaming holes. And although many consider power downfeeding on a Bridgeport to be a boring-only proposition, that’s not the case. By applying a flood of sulfur-based oil, I have power-downfed more high-tolerance holes with chucking reamers than I would care to count.

Lathes present some unique reaming challenges. One of them is that lathe tools generally mount horizontally. This makes the use of a reamer/floating holder arrangement a somewhat dicey proposition. Horizontally mounted chucking reamers must limit the radial and/or angular float so that the potential eccentricity of the reamer’s centerline to the drilled hole does not exceed half of the tool’s chamfer. Likewise, if a reamer is held in a solid holder, the centerline error with respect to the spindle can cause a sizing problem.

Additionally, when drilling and reaming occur during different setups, the hole may be slightly eccentric to the axis of rotation. This creates problems for both solid and floating holders used on lathes. It is easy to imagine the undesirable dynamics of a reamer mounted with radial float, rotating like a crankshaft while attempting to finish a drilled hole that runs out to the spindle centerline. Anyone having to ream under these conditions should consider boring instead.

In some shops, small holes are reamed with standard industrial-grade drill presses. This presents a new wave of challenges. The typical drill press is equipped with a 3-jaw chuck whose runout causes machinists and manufacturing engineers to wince. Bearing error and imprecise depth control are additional input variables that must be controlled.

Good bearings, a mounted indicator and a precision drill chuck can limit the negative effects of these variables. But for the growing number of shops trying to meet Six Sigma quality goals, even these efforts won’t be enough to overcome the drawbacks of a drill press.

Measuring Up
Another important part of the reaming process concerns how finished holes are measured. Given the tight tolerances involved, even small errors in the accuracy or repeatability of the measurement system will significantly impact one’s ability to judge good parts from bad ones.

Let’s evaluate three common types of gages: plug, dial and air.

Plug gages have a number of drawbacks. First, the inspectors, machinists or assembly technicians must fish around a precision hole with a hardened steel gage that may destroy a hard-won surface finish. Second, plug, or “pin,” gages are only certified to an accuracy of 0.000040". Considering that engineers, inspectors and machinists are making quality judgements at the edge of a 0.0005" tolerance range, 40 millionths is quite a bit.

Perhaps the most glaring plug-gage shortcoming involves the geometry of the hole itself. If you have ever measured finely enough, you know that there is no such thing as a perfectly round or straight hole. Properly reamed holes tend to have an average out-of-roundness of about 0.000040". (The worst case I ever saw approached 0.0014".)

Every reamed hole I have measured with a true circular geometry gage has exhibited seven distinct sides. This means that a solid plug gage will only measure the minimum inscribed diameter of a seven-sided hole.

Compared to a plug gage, a dial gage diminishes the risk of mechanical damage to the bore and provides the variable measurement data that can be analyzed with common statistical tools. The downsides to dial gages are their dependency on operator “feel” when taking the readings, their ability to only measure at two or three points at a time and their capability of damaging the bore when the workpiece material is soft or the operator is inexperienced.

Air gages, though often touted as the solution to plug- and dial-gage problems, also have drawbacks. A standard air-gage spindle has its jets set 180° apart. So it misses the seven-sided geometric error in much the same way that a conventional micrometer misses the out-of-round condition of a centerless-ground OD. This phenomenon is often called “odd-lobing.”

While air gaging offers the advantage of exceptional resolution, thermal changes can adversely affect fine measurements—especially in aluminum workpieces. This degrades the operator’s ability to distinguish conforming and nonconforming part features.

Taking Control
Given the tight tolerances involved and the challenges of measuring accurately, how do you ensure the quality of a reaming process? In the aerospace industry, there are initiatives afoot to define quality in purely statistical terms. More specifically, many prominent aerospace companies have adopted the Six Sigma philosophy pioneered by Motorola.

While a thorough discussion of Six Sigma is beyond the scope of this article, its most basic concept is simple: “In God we trust; all others bring data.”

The first step in establishing such a program is to develop a document known as a Process Failure Modes and Effects Analysis (PFMEA). The goal of this exercise is to identify all possible sources of process failure. It also is an attempt to quantify the chance of these failures occurring, the chance of their detection and their expected severity. The best part of a PFMEA is the control plan. The goal is to achieve a more consistent output by limiting the variable aspects of the process.

PFMEA may seem like a tool that would require a flock of engineers to implement and eat up about two weeks of time you don’t have. That doesn’t have to be the case.

If you own or manage a machine shop, I suggest you take your machinists out to a local watering hole, buy them a beverage or two and ask them this simple question: “What could possibly go wrong when you ream a hole?”

Make sure you bring a pencil, a pad and a strong wrist, because you’ll need to write quickly and, probably, for quite a while.

Space limitations prevent me from discussing every impediment to the reaming process that you’re likely to hear. But I want to focus on one that machinists tend to identify: the reamer manufacturer. This important element of controlling the process often is overlooked.

When it comes to your source for reamers, I suggest you do the following:

• Control the source. Test a variety of reamers, identify the best tool and then stick with the manufacturer of it.
• Survey the source. This approach is not for the faint of heart. You must gain admittance to your cutting tool manufacturer’s facility. Look for the process controls that are in place and the statistical tools that your toolmaker uses. Ask hard questions about how the company measures the key characteristics of its products.
• Inspect tools in-house. Some users of cutting tools in this country measure the key characteristics of every tool that lands on their dock. This sounds silly until you add up all the time and money that many businesses spend arguing internally and quibbling with suppliers about things such as the actual size and finish of reamed holes.

If you decide to inspect reamers in-house, use a precision spin-roll device to check straightness, runout between diameters and indicator drop over the reamer margins. Spin-roll devices cost anywhere from a couple of hundred dollars to a couple of thousand.

Whoever performs the inspections will need certain measuring skills. He or she will be working with an electronic or mechanical instrument that has a resolution as small as 0.000010". A good-quality indicating micrometer is required to assess the reamer’s functional diameter. A control chart must be constructed to allow the collected data to be documented and analyzed.

The setup parameters for your reamers will also play a large role in your control plan. Don’t let a $300,000 machining center wait for a properly setup tool. Preset all of your tools offline. Ideally, presetting equipment should be located within each work cell.

Define your runout parameters based on data, not generic recommendations from the manufacturer. For the reamers discussed here, 0.0002" to 0.0010" is a good place to start.

If you expect to consistently generate holes to a 0.0005" tolerance, you must track the collected reaming data on control charts. It must include preset control limits that trigger corrective actions. Develop a troubleshooting guide derived from the information obtained by constructing the PFMEA document.

If your organization fosters a culture of continuous improvement, ongoing efforts will eventually lead to better process capabilities and a reduction in the number of reamed features that must be inspected. Learn the capabilities of your tools and processes, control the inputs and watch as the number of unacceptably reamed holes decreases at your company.

About the Author
Mark Richardson is a manufacturing engineer at a Midwest producer of aircraft components.