Difference between revisions of "Endmills"

From ShapeOko
Jump to: navigation, search
(End Mill Selection Guidelines)
m (Mounting an endmill: Replacing Silicon with Teflon - silicon (and silicone) don't make sense in this context)
Line 148: Line 148:
==Mounting an endmill==
==Mounting an endmill==
Follow the spindle manufacturer's instructions. If necessary, consider using a bit of plumber's silicon thread tape or some other material on the collet of your rotary tool, esp. on the low-end tools.[http://blog.inventables.com/2013/11/milling-aluminum-with-shapeoko-2.html?utm_content=buffer5437c]
Follow the spindle manufacturer's instructions. If necessary, consider using a bit of plumber's Teflon thread tape or some other material on the collet of your rotary tool, esp. on the low-end tools.[http://blog.inventables.com/2013/11/milling-aluminum-with-shapeoko-2.html?utm_content=buffer5437c]
See [[Calibration_and_Squaring_the_Machine#Squaring_the_Spindle|Calibration and Squaring the Machine: Squaring the Spindle]] for techniques to mount it plumb.
See [[Calibration_and_Squaring_the_Machine#Squaring_the_Spindle|Calibration and Squaring the Machine: Squaring the Spindle]] for techniques to mount it plumb.

Revision as of 20:11, 22 December 2014

Endmills are cutting tools designed so as to be able to cut in the X- and Y- axis when mounted in a spindle. Some are also able to cut when plunging along the Z-axis (Centercutting), while others cannot (Non-centercutting).

One consideration for endmills is the tolerance to which they are made and how the actual diameter relates to the nominal diameter. Arguably the best way to handle this is to cut a slot or a shape and measure the result, but one may wish to start by measuring the endmill itself, esp. if one is using a spindle w/ very low runout.

There is a direct correlation between price and quality and tool longevity. While one should not expect a cheap bit to perform well, one also should not spend excessively on high-end bits when first beginning, given the possibility of destroying the bit through accident or mis-use.

Tooling life is measured in linear inches.[1]

End Mill Selection Guidelines

All other things being equal:

  • Length
    • Shorter endmills are more rigid, less-expensive and may provide a better finish (as a corollary, one should expose only the length of endmill beyond the cutting edge which is absolutely necessary[2])
    • Longer endmills, while not as rigid, afford the ability to cut more deeply, are more expensive and may not provide as nice a finish and may increase runout (see above note)
  • Number of flutes
    • One, two or three flutes are esp. suited for slotting or heavy stock removal
    • Four or more flutes provide a nicer finish and greater tool rigidity
  • Diameter
    • Larger diameter tools are more rigid and will clear more material in a given pass
    • Smaller diameter tools will have a smaller radius at corners and allow one to remove less material when profiling or cutting out parts
  • Materials
    • There is a direct relation between expense and tool life
  • Coatings
    • Coatings will allow higher feeds, speeds, and will extend tool life
    • Certain coatings will prevent material from adhering to the bit[3]

Forum discussion here: Recommendation for End Mill and Dw660

The best starting point is the default 2-flute, square-ended, straight-cutting (able to center-cut) 1/8" high speed steel (or solid carbide) endmill w/ no coatings.[4] One should move away from that baseline as is dictated by the materials which you are cutting, and the fashion in which you wish to mount them in the work-area, and the quality of cut which you expect. Switching to a spiral up-cut endmill for better chip ejection is an obvious choice (to the detriment of cut quality and increased chipping at the top surface when cutting plywood).


A wide variety of materials are used for endmills.

High Speed Steel (HSS)

High speed steel is commonly used when a special tool shape is needed, not usually used for high production processes. Inexpensive, at the cost of tool life.

Cobalt (M-42: 8% Cobalt)

An improvement over high speed steel. Reduced chipping under severe cutting conditions allowing the tool to run faster than HSS.

Powdered Metal (PM) Cobalt

Cost-effective alternative to solid carbide.

Solid Carbide

Able to run much faster than other materials, carbide is especially well-suited to use with rotary tools for general usage. Incredibly tough and long-lasting, it is brittle and subject to chipping, so should be handled with care. Carbide inserts are the most common because they are good for high production milling.


Usually used to make large-diameter tools.


An End Mill cutter with two flutes

Depending on the material being milled, and what task should be performed, different tool types and geometry may be used. For instance, when milling a material such as aluminium, it may be advantageous to use a tool with very deep, polished flutes and a very sharp cutting edge. When machining a tough material such as stainless steel, however, shallow flutes and a squared-off cutting edge will optimize material removal and tool life.

Non-optimal geometry will create results similar to a dull bit, e.g., fuzzy cuts in softer species of wood. Making a final finishing pass may help, another alternative is to spray a clear finish on the wood, allow it to dry and then re-run the finishing pass (the sprayed finish will soak into the wood and harden it).

End mills are described using a number of characteristics:


  • Square End --- general purpose, will cut a slot with square corners
    • Fishtail --- The tips of the cutting edge extend down past the center of the bit, making it especially suitable for punching through thin materials or cutting fine details[5]
  • Radiused --- general purpose, has corners slightly radiused so as to not cut a perfectly square corner (see below)
  • Ball End --- special purpose, will cut a slot with a rounded bottom. The radius will result in a stronger part, and will allow for more control over the shape of a pocket, but will require a large step-over value to avoid a scalloped appearance.
  • V-cutting --- special purpose, used for engraving. Identified by the angle of the V --- 90 degree bits can be used for mitering. Sharper angles will cut deeper for a given width of cut. See also V-carving reference books.
    • If work cannot be completed in a single pass, some operators will grind the tip to a 0.5--1mm radius ball point so as to minimize stepping (esp. when cutting wood)
    • # of Passes --- Size guidelines for adding a radius at the tip (may vary based on bit angle and material):
      • <10mm --- one pass
      • 10--20mm --- ~0.5mm
      • 20--35mm --- ~0.75mm
      • >35mm --- 1mm radius
  • The tradeoff is feature size vs. feature depth --- an acute angle allows one to cut a smaller, finer feature w/ more depth, while a more obtuse angle allows one to cut a larger area w/ a single pass and while having a single bottom, as opposed to a ragged set of scallops.
    • Recommended bit angle for a given text size:
      • <1" 45--60°
      • 1--2" 60°
      • 2--4" 60--90°
      • 4--6" 90°
      • 6--10" 90 to 120°
      • >10" 120° or greater
    • Material guidelines:
      • hardest timber available
      • use conservative plunge and feedrates when doing more than one pass
      • avoid overlapping V-cuts --- tends to cause splintering at the top edge, leave a ~0.5--1mm gap at the top
      • use a cutter w/ centered/symmetrical geometry
    • Formula for calculating the effective diameter of a V-bit at a given depth in Excel this is:[6]
=TAN(RADIANS(B3)) * B4 * 2

End Cut Types

Discussion in the forums: Advantages of non-center-cutting endmill?

  • Centercutting --- one or more cutting edges at the tip to allow plunge, drill or ramp movement into a cut. Most flexible, best-suited for general-use.
  • Non-Centercutting --- only capable of side (radial) cut or contour cutting into an exterior surface. Special-purpose, only suited for applications where plunge cutting is not necessary.

Similarly, flute geometry is available in several different forms:

  • Straight --- general purpose cutting --- will not cause as much chipping at the top as an up-cut spiral
  • Spiral
    • up-cutting --- pulls up on the work-piece, pulls the bit and the machine down into the cut --- affords the best possible chip ejection --- may cause chipping at the top surface on some materials
    • down-cutting --- pushes the work-piece down, and won't lift up thin materials --- poor chip ejection may result in re-cutting of waste material, dulling the bit, cleaner top edges on shallow pockets[7]
    • combination --- bottom portion of the cutting area is up-cutting and the upper portion is down-cutting, resulting in a better edge finish in materials which chip easily such as plywood.

Spiral cutting flutes may also vary in their geometry by the angle at which the helix works its way up the shaft of the tool. Shallower angles are used for roughing, while sharper ones are used for tooling intended to create a fine finish.

Number of Flutes

flutes performance

Single Flute

Largest possible flute space allowing for the greatest possible chip carrying capacity. Used for aluminum and plastics on commercial machines, is well-suited for plastics on less-rigid equipment.

Two Flute

Largest possible flute space in a symmetrical design. Used primarily in slotting and pocketing of non-ferrous materials where chip removal is a concern on commercial machines, is well-suited for general usage on less-rigid equipment.

Three Flute

Similar flute space to two flute designs, but having more material and greater rigidity.

Four/Multiple Flute

Used for peripheral and finish milling on commercial machines. The additional flutes allow faster feed rates, but chip removal may be problematic. Provides a much finer finish than tools with three or fewer flutes.


In the early 1990s, use of coatings to reduce wear and friction (among other things) became more common. Most of these coatings are referred to by their chemical composition, such as:

  • Titanium nitride (TiN) (a basic yellowish coating that has fallen out of wide use)
  • TiCN (a popular bluish-grey coating)
  • Titanium aluminium nitride (TiAlN and AlTiN) (an extremely popular dark purple coating)
  • TiAlCrN, AlTiCrN and AlCrTiN (PVD coating).
  • PCD veins. Though not a coating some endmills are manufactured with a 'vein' of polycrystaline diamond. The vein is formed in a high temperature-high pressure environment. The vein is formed in a blank and then the material is ground out along the vein to form the cutting edge. The tools can be very costly, however can last many times longer than other tooling.

Advances in endmill coatings are being made, however, with coatings such as Amorphous Diamond and nanocomposite PVD coatings beginning to be seen at high-end shops.

Milling Formula

  • 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): Number of revolutions the endmill makes in a minute

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

Chip Load: The amount that each flute cuts during a single revolution of an endmill

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

Mounting an endmill

Follow the spindle manufacturer's instructions. If necessary, consider using a bit of plumber's Teflon thread tape or some other material on the collet of your rotary tool, esp. on the low-end tools.[8]

See Calibration and Squaring the Machine: Squaring the Spindle for techniques to mount it plumb.

Total Indicated Runout Considerations

Another consideration is the interplay between bit diameter and the TIR (Total Indicated Runout) of a given spindle. If it is a significant portion of the end mill's diameter, the possibility of breakage increases significantly. Unfortunately, rotary tools often suffer from significant lack of concentricity in their bearings and other internals which often increases with wear/usage (see the Spindle Options page for further information and other options).

Technique for measuring runout: Measuring spindle runout with a dial test indicator.


Some materials require cooling when milling, various liquids are popular, but must be matched to the material.

Other materials require care when using liquid coolant, since the dust from milling is abrasive. Such materials often use air cooling as discussed in, Use of air cooling and its effectiveness in dry machining processes. One source of tooling to support that is Vortec vortex tubes.


As tough as they are, the edges of an endmill are very delicate and must be cared for as you would any fine tool. Always store them in their case when not in use.

Maintenance and Usage

While one must view endmills as a consumable item, they are also a fine piece of tooling. It is possible to sharpen certain endmills (but the companies which do so have a rather large minimum quantity for doing so). Another possibility is the old shop tradition of using used tooling for rougher work, or materials which do not require the same sharpness, then switching to a newer, sharper tool for a finishing pass.[9]


High Speed Steel and Carbide are both welcome at recyclers and should be carefully recycled once one has a sufficient quantity of material to make a trip worthwhile.

Specific Bit and Brand Recommendations

The following bits have been used by specific users as noted below.

If one is using a spindle or router w/ a 1/4" (or larger) shank, one may also use some standard router bits if one's workpaths are appropriate to their use[23]:

As well as end mills

Specific brand recommendations / notes:

  • V-bits
    • Insert bits --- Amana and Gerber are noted as being the only large diameter bits which balance properly
    • Kyocera bits work well for one pass work
    • Onsrud bits work well

Bits which have received positive mentions and may be worth investigating:

See the Endmills section of the Vendors page for a comprehensive listing of sources.

There is also a recommendation here.