High

Let’s get one thing straight from the start. I don’t give much of a hoot about the parts you make. But I do care very much about the chips, and you should too.

At the end of a machining process, you have two things: a finished part and a pile of chips. Most people focus on the part. I focus on the chips.

It’s not about being contrary. I believe if you produce a lot of really good chips, really fast, you can make a lot of money machining parts. There is a lot of fuss about the pluses and minuses of high-speed versus high-feed milling. While they are very different, in many respects they have similarities. But to be clear, it’s still all about the chips.

What two things does it take to make a chip? Heat and pressure. Metal cutting is a process of plastic deformation. Heat is created by the friction at the shear zone. Regulating the amount of heat is the rotational speed of the cutter. Pressure is generated by the feed. It is important to note the heat and pressure required to plastically deform the material and shear it away is the same heat and pressure that causes tool wear and premature failure. We want to direct the heat into the chip, but first we must have a thick enough chip to absorb the heat. That is where the high feed rates come from in high-feed milling.

All high-feed milling cutters, solid and indexable alike, have one very important factor in common: very large lead angles. The cutting edge on high-feed cutters can be straight or have a very large radius. But either way the resulting average lead angle is very high, usually somewhere between 78° and 82°.

What impact does a high lead angle have on the chip? As the lead angle on a milling cutter increases from 0° (square shoulder) to 45° or 75°, things start to happen to the chip. At 0° your chip thickness is equal to your feed per tooth. As the lead angle increases, chip thickness decreases. You can calculate your actual chip thickness by multiplying your feed rate IPT (inch per tooth) by the cosine of the lead angle. So, a .010” (0.254 mm) IPT feed rate, using a 78° lead angle would result in a 0.002” (0.0508 mm) actual chip thickness. That’s thin, and not nearly thick enough to absorb any heat. Your feed rate must always be greater than your edge preparation hone or T-land, or you turn your milling cutter into a piece of sandpaper. To achieve a 0.010” (0.254 mm) chip thickness using a 78° lead angle tool, you will need to program an IPT of .048” (1.22 mm). That is a 385 percent increase in feed rate, hence the name high-feed milling.

The high-feed rates achieved with high-feed milling do come with one tradeoff. Due to the large lead angles, their DOC (depth of cut) capabilities are limited. Maximum DOCs for most high-feed mills range between one and two millimeters. There are a few indexable exceptions to this rule that incorporate large IC inserts. Justifying the increased cost of such mills is that they can be three to four times faster than normal.

In addition to the productivity gains there is one other huge benefit to high-feed milling. It’s all about the force.

Another golden rule of milling is that cutting forces are always perpendicular to the cutting edge. High-feed cutters with an average lead angle between 80° and 82.5° generate some of the lowest radial forces in milling. Almost all the cutting forces are directed axially up into the spindle. The greater the ratio of axial to radial forces, the more stable the operation is. This can be an advantage, especially when tooling setup or part configuration requires a large gauge length. Long reaches and deep cavities are not an issue with high-feed milling. Gauge lengths on the magnitude of 10:1 (length to diameter) are common, but may require moderating the feed rate.

There are a few other application techniques to consider when high-feed milling. Keep as much of the cutter diameter engaged in the cut as possible. This will balance the axial forces generated by the high lead angle. As the ae (radial width of cut) decreases and approaches 50–60 percent of the cutter diameter, stability diminishes. Care should also be taken when programing your cutter path. At high feed rates, smooth transitions in cutter path direction are preferred. Avoid 90° turns at all costs as they create excessive radial engagement, meaning high radial forces and chatter. Program an arc or radius in corners at least 50 percent larger than the cutter diameter when changing directions. Remember, transitioning from a straight-line move to an arc means reducing your feed rate. In the example provided above, you would reduce the feed rate by 33 percent.

The formula used to determine the corner or circular interpolation feed rate compensation is: ((2 × arc radius) – cutter diameter)) / (2 × radius).

In summary, high-feed milling is all about chip thinning. You must increase feed rate to compensate for the chip thinning created by the large lead angle, typically 80° to 82.5°. In most cases your feed rate is four to five times faster than standard feed rates utilizing square shoulder or 45° lead milling cutters. The large lead angle, while somewhat limiting the axial DOC, pushes most of the cutting forces axially up into the spindle, increasing stability, and allows for long reach capabilities.

Just as in car racing, care must be taken when entering corners and changing cutter path directions. Use the feed-rate compensation calculation to reduce your feed rate and use smooth arcs or radius tool paths when changing directions to prevent excessive cutter engagement and chatter. Applied correctly, high-feed milling is a productive metal-removal process and can be a lifesaver in deep-cavity and long-reach applications.

Like high-feed milling, high-speed milling also means increasing your feed rate to compensate for chip thinning, but not because of the tool’s lead angle. Chip thinning in high-speed milling results from limited radial engagement of the cutter diameter in the cut. In turning, the chip has a constant thickness. A milling cutter, however, cuts on an arc, not a flat plane. Chip thickness varies depending on where the cutting edge is in relation to the arc of the cut. When a milling cutter diameter is fully engaged in the cut the chip thickness is zero on entry and exit and at its thickest in the middle of the arc of rotation. As with all metal-cutting operations, we must manage chip thickness and remember chip thickness is not always equal to feed rate.

We first introduced the concept of chip thinning when we discussed lead angle. As lead angle increases, chip thickness begins to thin. In a normal turning operation, once the chip thinning factor for the lead angle is applied, chip thickness remains the same.

Milling requires factoring in both the chip thinning for lead angle and chip thinning for radial engagement. The result is called “average chip thickness” or hm. Now, before any physics majors go off on me, hm is a physics term meaning the measure of the point in the middle of the group. Average is just that; the average of the entire group. I do not know why the metal cutting industry decided to conflate the two, but they did, so I will continue the charade.

Please note that the chip thickness is zero at the beginning, middle and end of the cutter rotation in the cut. The chip is the thickest on the centerline. The average hm is located between the centerline of the cut and the beginning and ending of the cut.

So why do we care about the average chip thickness? Remember: What does it take to make a chip? Heat and pressure. You want the heat to go into the chip. This is where average chip thickness (hm) comes into play. Average chip thickness must be greater than edge preparation, T-land or hone, or again the milling cutter becomes sand paper. Carbide likes to cut; it does not like to rub. Rubbing creates uncontrollable friction and heat that is detrimental to the life of your tool. This is where the feed per tooth equation comes in: fz = hm × √(D1/ae) × cos(K).

This equation looks difficult but it’s not—and it makes all the difference between success and failure.

The key to high-feed milling is understanding the relationship between the radial engagement (ae) of the tool and the impact it has on the average chip thickness (hm) and programmed feed rate per tooth or flute fz. As the radial engagement of the cutter diameter is reduced, your programmed feed rate must be increased to compensate for the radial chip thinning that will occur. By using the formula, you may calculate the programmed feed rate fz required per flute or insert to achieve the desired average chip thickness (hm). Most cutting tool manufacturers provide both the fz (feed per tooth) as well as the hm values based on the size and shape of the edge preparation for the given tool. Once you have calculated the required feed rate per flute or insert calculating the IPM (inches per minute) table travel is easy. In most cases, IPM feed rate will be more than four or five times faster than standard feed rates.

In high-feed milling, the high feed rate is coupled with high axial depth of cut and specific cutter path strategies to achieve high metal-removal rates. The higher axial depth of cut is possible due to the reduced radial forces created by the reduced radial engagement. Typically, axial depths are greater than two times the diameter and up to six times diameter is achievable. Radial forces can be further reduced by using a higher helix angle, which drives more of the cutting force into the spindle. Chip evacuation at the higher axial depth of cut is not an issue because the chips are not crowded into the flute as they would be with a higher radial engagement. The ease of chip evacuation also allows the use of tools with more flutes or inserts, resulting in even higher feed rate capabilities. Tools with more flutes and inserts typically have larger core diameters due to small chip gullets or flute spaces which further enhances stiffness, rigidity and stability.

In addition to these benefits, high-speed milling also reduces the amount of heat transferred into the tool and the part, enhancing tool life and reducing the possibility of work-hardening the part. It is counter-intuitive; when you hear high speed, you think high heat. Not true here. In a full slot application, the full diameter of the cutter is engaged in the workpiece or the cutter has a full 180° arc of engagement. This high arc of engagement means the cutting edge is engaged in the cut a long time, thus producing more heat. As the radial or arc of engagement decreases so does the amount of time each cutting edge is in contact with the workpiece, producing less heat and providing the cutting edge more time to cool between cuts.

This reduction in heat has a couple of benefits. It helps prevent work hardening in high carbon and stainless steels and reduces the amount of heat transfer back into the tool when machining refractory metals and super alloys. Bottom line: it enhances tool life. With all these positive outcomes, what’s the catch?

There is no real catch, however, there are basic principles that need to be followed. Rigidity of the entire machining mechanism: the machine, spindle, holder, fixture, etc., is always important. Keeping a constant load on the tool is key and requires specific tool paths—no sudden, sharp directional changes.

Trochoidal milling, dynamic milling, volumetric milling, or slicing are a few cutter-path strategies supported by most modern CAD/CAM software that aid high-speed and high-feed machining. In many cases, it takes a combination of more than one strategy to complete the part.

Remember, the more chips on the floor, the more parts out the door!

Connect With Us