BORING ON THE MILL

Introduction

Boring on the mill is a simple operation in theory, but requires close attention to detail for success when precision is important (i.e. to within 0.001” of target size).

*** CAUTION ***

Please understand that using a boring head on a milling machine is an inherently dangerous process because the tool is deceptively dangerous when rotating, so YOU MUST KEEP YOUR HANDS AWAY FROM THE CUTTING ZONE AT ALL TIMES WHEN THE MILL IS RUNNING.

Step 0: Understand EVERYTHING Matters

Using a boring bar to simply enlarge an existing hole is a straightforward process. However, when trying to hit a particular size and tight tolerance, everything begins to matter: boring bar selection and setup, cutting edge geometry, tool deflection, lubrication, cutting parameters, chip evacuation, part temperature, and our ability to measure the bore accurately and precisely. If you cannot force yourself to be a little OCD, you might not be good at precision boring J.

Step 1: Boring Bar Selection

There are three general types of boring bars: high speed steel, brazed carbide, and indexable carbide. The benefits of HSS are that it is cheaper and tougher. The benefits of carbide are that it can tolerate much more heat (i.e. it can cut 2.5 – 5 times faster than HSS), and it has a modulus of rigidity that is about 2.5 times greater than steel.

Figure 1: Examples of HSS boring bars.

Figure 2: Example of brazed carbide boring bars, where a small piece of tungsten carbide is brazed onto a cheaper steel shank. When the carbide chips, the boring bar is either reground (which is difficult to do well) or discarded.

Figure 3: Example of indexable carbide boring bars, where a replaceable tungsten carbide insert is attached to a machined pocket in a steel or carbide boring bar shank. When the carbide insert chips, it can be easily and quickly rotated to another corner (indexed) or replaced with another insert.

Figure 4: Larger corner radii are stronger and better for roughing, but smaller corner radii typically produce more accurate bore sizes and better surface finishes (at reduced feeds).

As with all metal cutting processes, stiffness is key when boring, so do everything you can to maximize it: use the largest diameter boring bar and the shortest clamping length possible.

Step 2: Boring Bar Setup

It’s worth repeating: as with all metal cutting processes, stiffness is key when boring, so do everything you can to maximize it: use the largest diameter boring bar and the shortest clamping length possible.

Figure 5: Example of properly selected brazed carbide boring bars. Notice how short and stiff the selected bars are in relation to the respective workpieces.

Many boring bars do not have alignment flats on them, so it is necessary to orient the top (flat) surface of the cutting edge so it passes through the centerline of the spindle axis, as shown in figure 6. This orientation is referred to as a neutral rake angle and is the safest for most materials and the only orientation that works properly when using these types of boring bars in a boring head. When setting a boring bar with no alignment flats, it is always necessary to perform a test cut to ensure the rake angle is set properly.

Figure 6: Examples of possible boring bar orientations (negative (left), neutral (center), and positive rake (right)). ALWAYS use neutral orientation (center) in a boring head on a mill.

When setting up the workpiece, always ensure adequate clearance exists beneath it and the vise if boring a thru hole. Whether boring a thru or blind hole, always set the quill depth stop appropriately to prevent an over-travel condition, which would damage the part, the boring head, and potentially the vise.

Figure 7: Set the quill depth stop before using the boring head.

Step 3: Selection of Cutting Parameters

When using a boring head on a milling machine, it’s best to begin with a cutting speed equal to half the typical computed value and work your way up if vibration and tool life allow it. The primary reasons are the reduced stiffness due to the cantilevered nature of boring bars, as well as the difficulty of providing consistent lubrication to, and chip evaluation from, the cutting edge of the tool unless flood cooling, as in a CNC mill. For safety reasons due to the rotational imbalance inherent in a boring head, never rotate the boring head faster than 600 rpm in the design lab.

Boring heads on Bridgeport-size milling machines should usually not be used with depth cuts deeper than 0.020”. It’s important to understand there is also a safe minimum depth of cut, below which the tool constantly transitions between cutting and smearing, leaving a very inconsistent size and finish. This safe minimum depth of cut is typically around 0.003” to 0.005” depending on the material. Harder / stronger materials can usually tolerate a smaller minimum depth of cut, as can boring bars with sharp corners.

When making depth adjustments, you can use the calibrated dial on the boring head, or a dial indicator if trying to be as precise as possible, or using a worn boring head.

Figure 8: Example of using a dial indicator to adjust the boring head depth of cut. This isn’t always necessary, but it facilitates more accurate adjustments.

Step 4: Bridgeport Automatic Quill Feed

Bridgeport milling machines have three choices for quill automatic quill feedrate: 0.001, 0.003, and 0.006 in/rev. The middle speed typically works well for most work.

The following schematic and accompanying video explain the function of the automatic feed.

Figure 9: Bridgeport automatic quill feed explained. Click for short video illustrating its use.

Step 5: Ideology for Repeatable Results

Consistency is crucial to obtaining repeatable results when using boring heads. Meaning, you want to vary the fewest parameters possible during each cut, and preferably only one at a time. Anything that affects the cutting force at the tool tip will change the amount of material removed, or the surface finish obtained: depth of cut, feedrate, lubrication, corner radius, part temperature, etcetera.

Let’s say you are trying to thru-bore a 1” hole in a piece of 303 stainless steel. One approach would be as follows:

1. Remove as much material as possible by drilling, since it’s the most efficient method of material removal. When doing this, be sure to leave enough stock for the next step. Leave the bore about 0.050” small in this case.

2. Perform a few test cuts to check how the boring bar is cutting. Rarely will a boring bar cut perfectly. If you try to remove 0.010” off the diameter of the bore, it may only remove 0.0096” on the first pass and another 0.0004” on the spring pass. (A spring pass is simply a second pass that helps compensate for tool or part deflection during the first pass.) It’s important to make a couple passes and write down how much each removes so you can take the average and know what to expect when it matters.

3. Do not try to “sneak up” on the final size. As anti-intuitive as it may sound, the best results are not obtained by making smaller and smaller cuts until you reach the desired size because of the safe minimum depth of cut discussed in Step 3 above. The best results are obtained by repeatedly removing a similar amount of material on each pass and using the resulting measurement data to make small adjustments to each subsequent pass. On the 1” 303 example piece, the final cut would remove 0.005” to 0.010” from the diameter to bring the part into final size tolerance.

Step 6: Bore Measurement

Bore measurements can be made using several tools, depending on the budget, operator skill, and required measurement accuracy.

Dial or Digital Calipers

The easiest tool to use for bore measurement is also the least accurate: dial calipers. These typically aren’t very accurate (within a couple thousandths of an inch) on smaller bores because the inside jaws have flats ground into them that prevent them from measuring the true size of the hole.

Figure 10: Measuring larger bores with dial or digital calipers.

Inside Micrometers

The second easiest tool to use is an inside micrometer. However, inside mics typically only work well for measuring shallow bores up to approximately 3” in diameter. They are accurate to +/-0.001”.

Figure 11: Inside micrometers used to measure a precision bore.

Small Hole Gages

Next are small hole gages, which are also inserted into a bore until a small amount of drag is felt and subsequently measured with outside mics. Used in sensitive hands, small gages are accurate to +/-0.002”.

Figure 12: Example of small hole gages.

Gage Pins

Gage pins are another way to measure precision holes. Gage pins are available in virtually any size and typically manufactured (precision ground) to +/-0.0002” tolerance.

Figure 13: Gage pin assortment used to measure precision bores.

Telescoping Gages

Telescoping gages are commonly used to measure bores, but require a lot of operator skill to provide repeatable and accurate results. After being inserted into the bore, a small amount of torque is applied to a friction lock, the telescoping gage is swept through the center of the bore, and subsequently measured with a micrometer. The challenge is applying the proper amount of torque to the friction lock, as too little results in the gage not holding the true bore reading once removed, and too much results in the gage distorting and showing a reading that is larger than the actual bore size. Like all metrology tools, practicing on a bore of known size (like a bearing race for example) is the only way to become proficient in the use of telescoping gages. Used in sensitive hands, telescoping bore gages are accurate to around +/- 0.0015.

Figure: 14: Using telescoping gages and outside mics to measure bore diameters.

Bore Gages

Bore gages are essentially precision telescoping gages with dial indicators built in. In use they are first calibrated using an outside micrometer and then the actual bore size is measured relative to that calibration using the dial indicator . Bore gages are accurate to +/-0.0005”.

Figure 15: Bore gage used to measure the bearing diameter of a connecting rod for an automobile engine.

3 Point Micrometers

The best tool for accurately measuring bores is a 3 point internal micrometer; however, these are also the most expensive option because each has a limited measurement range, so several units have to be purchased to cover a decent range of sizes. 3 point micrometers are accurate to +/-0.00005” to +/-0.0001”.

Figure 16: 3 Point Bore Micrometers.

Miscellaneous Tips