The High Feed, High Reliability Process

When button cutters and high-feed mills are used properly, feed rate and confidence go hand in hand.


Facebook Share Icon LinkedIn Share Icon Twitter Share Icon Share by EMail icon Print Icon

To realize a process that is better suited to run unattended, try turning up the feed.

Seriously. Almost anyone would assume that a lower feed rate makes the process more reliable, and therefore better suited to let the operator step away from it to perform some other task. But certain types of milling cutters—most notably high-feed mills and button cutters—can cut with greater reliability and productivity when the feed rate is increased.

Don Yordy, die/mold milling product manager for Ingersoll Cutting Tools, says the proper application of these tools deserves to be better understood. Shops he has worked with in die/mold applications have achieved high-feed, high-reliability processes with these cutters. But the principals involved can apply just as well in various applications where the machining center has some additional feed rate available to put to use.

Button cutters and high-feed mills are inserted milling tools with circular edges. A button cutter uses inserts that are round. What Mr. Yordy calls a high-feed mill uses inserts that are only partially round, with a large radius defining the cutting edge's curve.

How this round cutting edge relates to unattended machining is best explained in a series of four steps.

1. A round insert converts radial cutting force into axial cutting force as the depth of cut gets smaller.

Figure 1 illustrates this. The round profile redirects the cutting force vector as depth of cut decreases. At a lighter cut, a greater proportion of the cutting force is directed "up," or parallel to the spindle axis.

2. Directing the force axially reduces vibration.

Radial force tends to deflect the tool, resulting in a process that is prone to vibrate, and therefore prone to cause a carbide tool to fracture. But axial force can make the process less susceptible to harmful vibration. The axial force places the assembly of tool and toolholder in compression. Instead of fracturing, the stability that results encourages the tool to fail through gradual edge wear.

3. The more stable cut is more predictable.

That change in the mode of tool failure is the key to unattended machining. A tool that might fracture at any time needs an operator standing close. But gradual wear is predictable. A process limited by wear instead of fracture makes it possible to predict with confidence when the operator who has stepped away must return to the machine.

4. Chip thinning permits a high feed rate, keeping productivity high.

The more predictable milling is no benefit if the light depth of cut results in low productivity. A high feed rate is needed to compensate for the light depth. One phenomenon that helps in this is "chip thinning." When using a round cutting edge at a shallow depth of cut, chip thinning produces a chip thickness that is less than what the programmed rate of advance per tooth would suggest, as Figure 2 illustrates. The consequence of chip thinning is that a higher programmed feed rate corresponds to the feed per tooth intended for the tool. In other words, this style of milling demands an exchange of high feed rate for low depth of cut, and chip thinning is part of what makes that exchange possible.

The combination of all of the points above creates a daisy chain connecting high feed rates to unattended machining. To summarize: Confidence in unattended machining comes from predictable tool life...predictable tool life comes from axially directed cutting force...axially directed cutting force results from cutting at low depths with circular cutting edges...cutting at low depths with circular edges leads to chip thinning...and chip thinning makes possible the high feed rate that keeps the productivity high.

Mr. Yordy says a variety of characteristics can make the tool more effective for cutting in this way. They include:

  • TiAlN coating. This coating can perform better under the heat that comes from high-feed cutting. The inert aluminum oxide layer that develops has a high hot hardness, protecting the tool.
  • Positive rake. Thanks to a light cut, the tool no longer has to be designed to have the face of the insert leading the cut in order to protect the cutting edge from impact. A more positive rake can shear the material away instead of plowing it, potentially decreasing heat buildup in the material by letting the chip carry most of the heat away.
  • Harder substrate. In a deeper cut, the insert's substrate needs to favor toughness to withstand vibration. But the more stable cutting from axially directed force takes care of the vibration danger. The trade-off between toughness and hardness can be shifted to favor the latter. A harder substrate can be used, extending the life of the tool.

Chip Thinning: Understanding Programmed Feed Vs. Chip Thickness

When the depth of cut is less than the radius of a round milling insert, the chip thickness is less than the programmed feed advance per tooth. Figure 2 illustrates this. The phenomenon is called "chip thinning."

Chip thinning means that a higher programmed feed rate will be needed to achieve any particular value of chip thickness, measured in inches per tooth.

Ingersoll Cutting Tools' Don Yordy provides the following formula for determining the feed rate that corresponds to a given chip thickness when a round insert is used at a light depth. The formula only applies when depth of cut is less than or equal to the insert radius. Here, IPT is the intended chip thickness appropriate to the tool, DOC is the depth of cut and D is the diameter of the cutting insert. (Or if the insert is not fully circular, D is the diameter of curvature of the insert's profile.)

Using these variables, the feed rate that should be programmed is determined as follows:
Programmed feed rate per tooth =

Example: A shop is cutting with 1/2-inch-diameter button inserts at a depth of cut of 0.050 inch. The shop wants to realize a chip thickness of 0.010 inch per tooth.

The programmed feed in this example would be

. . . or 0.017 inch per tooth.

In other words, the programmed feed rate can be this much higher because of chip thinning. Without chip thinning, the shop trying to hold 0.010 ipt with four cutting edges at 2,000 rpm would be limited to 0.010 ipt × 4 teeth × 2,000 rpm, or 80 ipm. But the shop trying to hold the same effective chip load under the influence of the chip thinning described above could set a higher feed rate than this. The feed permitted here would be 0.017 ipt × 4 teeth × 2,000 rpm, or 136 ipm.

Technically, the phenomenon described above would more accurately be described as "axial" chip thinning. All of the discussion above assumes a full width of cut. But if the width of cut, or radial depth of cut, is less than the radius of the cutter, then a similar radial chip thinning applies.


  • Where Dry Milling Makes Sense

    Liquid coolant offers advantages unrelated to temperature. Forced air is the fluid of choice in this shop...but even so, conventional coolant can't be eliminated entirely.

  • Start With The Right Speeds And Feeds

    Running rotary milling cutters at the proper speeds and feeds is critical to obtaining long tool life and superior results, and a good place to start is with the manufacturer's recommendations. These formulas and tips provide useful guidelines.

  • Choose The Best Drill Point Geometry

    The more common twist drill point geometries often are not the best for the job at hand. By choosing the best point for the material being drilled, it is possible to achieve better tool life, hole geometry, precision, and productivity.