End Mills are used for milling, profiling, contouring, slotting, counterboring, drilling and reaming.

Cutting Tool Materials

High Speed Steel (HSS): Provides good wear resistance and costs less than cobalt or carbide end mills. HSS is used for general purpose milling of both ferrous and non-ferrous materials.

Cobalt (M-42: 8% Cobalt): Provides better wear resistance, higher hot hardness and toughness than high speed steel. There is very little chipping or microchipping under severe cutting conditions allowing the tool to run 10% faster than HSS, resulting in excellent metal removal rates as well as good finishes. This material, combined with the proper geometry has proven the most cost-effective for machining cast iron, heat treated steels and titanium alloys.

Powdered Metal (PM) Cobalt:A cost effective alternative to solid carbide, powdered metal is tougher and less prone to breakage. Tools perform well in materials < 30RC. PM is used in highshock and high-stock applications such as roughing.

Solid Carbide: Primarily used in finishing applications, carbide provides several advantages over HSS or cobalt materials. Carbide can run much faster because of the material’s extreme hardness. This allows the cutter to withstand high cutting temperatures and provides excellent wear resistance. Carbide also provides better rigidity than HSS, which enables the end mill to provide a higher degree of dimensional accuracy and superior surface finishes. Carbide provides the user with the ability to run faster with less tool wear. However, the user should be aware that carbide’s hardness comes at the expense of its toughness. Carbide is brittle and tends to chip when conditions are not ideal, rather than wear. Heavy feed rates are more suitable for HSS and cobalt tools. Carbide end mills, which can be run 2-3X faster than HSS, are best for maximizing speed and tool life.

Carbide-Tipped: Offering some of the advantages of solid carbide tooling, carbide is brazed to the cutting edges of steel tool bodies. This is particularly a cost-effective option for larger diameter tools.

End Mill Type

Finishing End Mills

Square End: Used for general milling applications

Ball End: Used for shallow slotting, contour milling and pocketing applications. Used to produce a radius in the bottom of slots or pockets for added strength. Also used to create compound curves for molds and dies where sharp corners must be avoided.

Corner Radius: End mill with radius ground on tops of flutes to help reduce chipping on the tip. These are best used for mold applications, removing more material faster than ball end mills.

Tapered: Results in faster and freer cutting due to more evenly formed chips over the entire length of the flute. Also has improved resistance to both operating side thrusts and deflections due to constant helix.

Roughing End Mills

In order to improve productivity over a conventional end mill, the roughing end mill (also know as a “hog mill”) was designed not to last longer, but to remove more material by taking heavier cuts in a fixed amount of time, without creating vibration. Ideal for today’s rigid and powerful CNC machinery.

Coarse Profile: This is the most commonly found profile. It is excellent in deep slotting conditions and heavy side cuts, and its design draws the least amount of power consumption. It is recommended for heavy machining conditions where high metal removal rates are required.

Fine Profile: Designed to increase tool life over a coarser profile, this style is recommended for profiling operations, but NOT in the following conditions: (Depth of Cut) x (Width of Cut) > Diameter squared (D2).

The fine profile has a shape, which provides the tool with a stronger edge that will last longer and permits a better surface finish on the workpiece. Works well in harder materials such as Inconel and Hastelloy.

Flute Types

Two Flute: The two-flute end mill has the greatest amount of flute space allowing for more chip carrying capacity. Used primarily in slotting and pocketing of non-ferrous materials where chip removal is a concern.
Three Flute: While this tool has the same flute space as two flutes, it has a larger cross sectional area providing for greater strength and the ability to pocket and slot both ferrous and nonferrous materials.
Four/Multiple Flute: Ideal for peripheral and finish milling. The additional flutes allow faster feed rates, but due to the reduced flute space, chip removal may be a problem. Produces a much finer finish than two and three flute tools.

End Cut Types

Centercutting: The tools have one or more cutting edges at the tip to allow the user to plunge, drill or ramp into a cut. This type of tool offers the user the greatest variety of applications.
Non-Centercutting: Peripheral teeth allow the user to side (radial) cut or contour an exterior surface. Used in applications where plunge cutting is not necessary.

Shank Types

Plain Shank: The most common, used in conjunction with a collet type holder
Weldon Shank: The shank of the tool has 1 or 2 flats with set screws in holder that tighten on flanks of flats to hold the end mill, preventing it from rotating.

Surface Treatments

TiN (Titanium Nitride): Provides extreme hardness and heat resistance allowing tools coated with TiN to run at higher speeds and feeds. Excellent for general-purpose use, TiN provides higher lubricity for freer chip flow, reduced buildup edge formation and cratering. Use caution on nonferrous materials because of a tendency to gall. Requires an increase of 25% to 30% in machining speeds vs. uncoated tools.

TiCN (Titanium Carbonitride): Harder and more wear resistant than TiN under conditions of moderate cutting temperatures. TiCN can provide the users the ability to run the job at higherspindle speeds (50% over TiN), especially in stainless steels. Use caution on non-ferrous materials because of a tendency to gall. Requires an increase of 35% to 50% in machining speeds vs. uncoated tools.

TiAlN (Titanium Aluminum Nitride): Ideal for conditions where extremely high temperatures are generated, TiAlN enables the users to increase the surface feet per minute (SFM), extend tool life and use less coolant. Ideal for stainless steel, high alloy carbon steels, nickel-based hightemperature alloys and titanium alloys. Use caution in non-ferrous material because of a tendency to gall. Requires an increase of 75% to 100% in machining speeds vs. uncoated tools.

AlTiN (Aluminum Titanium Nitride): Used for machining aircraft/aerospace materials, nickel alloys, stainless steel and titanium. Allows for aggressive speeds and feeds. Used in dry machining of cast irons, nodular iron and selected carbon steel. Requires an increase of 75-100% in machining speeds vs. uncoated tools.

Laser Coating: Used for high speed finishing and light metals such as aluminum. Laser works well in abrasive materials such as graphite, plastics, and high silicone aluminums. The laser coating provides twice the lubricity of TiN, extends tool life and reduces edge wear.

ZrN (Zirconium Nitride): Offers an improved finish when used in aluminum, brass, copper and other non-ferrous materials. Has a higher oxidation temperature than TiN, resists sticking of heated aluminum, increases lubricity and prevents "edge buildup."

Flute Centercutting tools

End Mill Selection Summary

  • Select the shortest possible end mill for the greatest rigidity
  • Select two or three flutes for slotting or heavy stock removal
  • Select multiple flutes for finishing and greater rigidity
  • Use the largest diameter possible for added strength and rigidity
  • Use cobalt, PM/Plus, and carbide for tougher and harder materials, and for high production applications
  • Apply coatings for higher feeds, speeds, and tool life

Common Milling Problems & Solutions

Excessive Chatter

Problem: Vibration and sound are excessive when the tool engages the workpiece

Possible Solutions:

  1. Increase your feed
  2. Reduce your cutting forces by reducing speed and/or feed or axial and/or radial depth of cut
  3. Increase your system′s rigidity by changing over to a stub length end mill or improving your workpiece fixturing
  4. Change geometry – use an end mill with variable flute spacing or a small circular margin

Poor Surface Finish

Problem: Work surface looks uneven and feels rough

Possible Solutions:

  1. Increase system rigidity
  2. Increase speed
  3. Reduce Feed
  4. Change to higher helix geometry
  5. Change to an end mill with more flutes

Excessive Wear of End Mill

Problem: Tool is wearing at cutting edges causing poor performance

Possible Solutions:

  1. Reduce Speed - A 50% reduction in speed will almost double the tool life
  2. Increase/Decrease Feed - A feed rate that is too light will cause excess rubbing
  3. Change Geometry of the Tool - Number of flutes, helix angle, length of cut
  4. Change material grade and/or add a coating

Milling Formulas

RPM = SFM x 3.82 ÷ Tool Diameter

IPM = RPM x # of Flutes x Chip Load

Chip Load = IPM ÷ RPM x # of Flutes

SFM = .262 x Tool Diameter x RPM

Revolutions per Minute (RPM):How many revolutions the cutter has in one minute

Inches per Minute (IPM): Number of inches the cutter passes through the workpiece in one minute

Chip Load:The amount that each flute cuts during a single revolution of a cutting tool

Surface Feet per Minute (SFM): This is the cutting speed of the end mill in the United States. It is the number of feet per minute that a given point on the circumference of a cutter travels per minute