BORING ON THE LATHE

Introduction

Like parting, boring on the lathe 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). For those who like to take notes as you read, here’s a condensed pdf version of this document.

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: one piece (left) and indexable (right). When the cutting edge wears or chips, it can be easily re-tipped on a standard grinder and honing stone.

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 extension 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 extension length possible.

Figure 5: Example of properly selected brazed carbide boring bar (left) and indexable carbide boring bar (right). 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 parallel to the XZ plane of the lathe, as shown in figure 6. The safest orientation is neutral (B) and if you elect to try a different orientation, be careful that adequate cutting tip clearance exists and that the tool tip is set on vertical spindle centerline. Positive rakes are used for cutting weaker materials like aluminum and plastics, and negative rakes are used for cutting stronger materials, like higher strength steels.

Figure 6: Examples of possible boring bar orientations (negative (A), neutral (B), and positive rake (C)).

Like all tools used on the lathe, boring bar tool height must be checked and adjusted so it is as close to the vertical spindle centerline as possible. Never assume the tool is setup properly just because it was in the lathe cabinet for the machine you’re using! If the boring bar is not on vertical centerline it will fail to cut properly, and will be damaged in use.

Figure 7: Example of ruler technique (left) and lathe gage (right) used to set boring bar vertical centerline height.

Step 3: Selection of Cutting Parameters

TIP: When using boring bars, 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 lathe.

TIP: A safe maximum depth of cut for a boring bar is twice the corner radius. 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 0.002” to 0.005” depending on the material. Harder / stronger materials usually can tolerance a smaller minimum depth of cut.

TIP: A safe maximum feedrate for a boring bar is one quarter of the corner radius.

Step 4: Ideology for Repeatable Results

Consistency is crucial to obtaining repeatable results when using boring bars. 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 5: 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 (0.5”) because the inside jaws have flats ground into them that prevent them from measuring the true size of the hole.

Figure 8: 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 about +/-0.0005”.

Figure 9: 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 +/-0.0005”.

Figure 10: 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 11: 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 +/-0.0005.

Telescoping gages can measure deeper bores than inside micrometers, which allows you to measure the amount of taper in a bore, not just the diameter close to the surface of the part.

Figure: 12: 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 13: 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 14: 3 Point Bore Micrometers.

Miscellaneous Tips