Tooling

To begin with, there are different tools that are used during the Machining process, each having a specified job.
The main three different tool types available are:

1. Drill Bits are designed to plunge directly into material, cutting axially, and creating cylindrical holes
2. Mill Bits are designed to undergo horizontal carving and cutting laterally.
3. End Mill Bits

In addition to that, there are many specifications related to tools that vary from bit to bit.Those are affected by the project type, material being cut, and the desired surface finish. A detailed discription of those specifications will be mentioned below.
Among those specifications are:

1. Diameter
2. Shank
3. Length of Cut
4. Overall Tool Length
5. Teath
6. Number of Flutes
7. Tip Shape represents the shape of the tip for the used tool.
8. Coatings
9. Center Cutting Capability means the ability to cut both axially and laterally.
10. Helix Angle
11. Helix Direction

The image below illustrates the different parts of a bit showing the Diameter, Shank, Length of Cut, Overall Tool Length, Teath, and the Flute.

Tip Shape

Concerning the Tip Shape of the End Mill, there are many different tip shapes that are designed for particular purposes. The most common shapes available are the following:

• Ballnose mills produce a rounded pass and are ideal for 3D contour work, because their rounded edge reduces jagged steps when cutting several stepped layers. Ball nose mills can also be used to cut wide paths with rounded edges by reducing the step over amount (overlapping distance between) between passes
• Fish Tail cutters are used to produce a flat surface.
• Surface Planing
• V-carving produce a “V” shaped pass and are used for engraving.
• Straight These bits are made to skim the surface and leave a smooth flat finish.

The image below illustrates the different tip shapes of a bit.

Material and Coating

Concerning the material, you should choose a bit made for the material of your choice. Many manufacturers make bits especial for your material of choice. Bits for hardwood are designed to leave a clean edge. Bits for plywood and laminates are designed so they won’t mangle the outer veneer layers. Bits for plastics are designed to avoid excessive melting. Aluminum cutting bits are designed to clear chips efficiently to avoid rewelding (heated chips getting fused to the hot cutting tool). Many bits can be used for multiple applications so you don’t need to buy 30 bits right away if you are in the prototyping stage of your project. A good all purpose bit is a 2-flute up cutting spiral bit.
There are many router bit material available and here are some of them:

1. HSS – High Speed Steel A tool steel far superior to carbon steel when used for drill bits and cutting tools. A HSS drill bit can drill a hole much faster than a carbon steel bit, hence its name. Quite the innovation in the 1940's! We've moved past this type of tool steel today, HSS bits are only suitable for cutting foams. (some disagreement here)
2. SC – Generally just called Solid Carbide. A very tough wear resistant steel. Many forms of Carbide exist (silicon carbide, tungsten carbide, Beryllium carbide, etc.) as do forms with different grain size. Solid carbide router bits can vary from worthless to extreme high quality.
3. Carbide Tipped – Carbide is expensive... larger diameter bits are available with chunks of carbide brazed (welded) to a steel body. This reduces the total amount of carbide used to make the bit and hopefully the price. Every thing above applies here. Generally, bits with .1" or more carbide thickness is considered a sharpen-able bit. Note: a sharpened bit may no longer be its full design diameter, and will need to be compensated for in the CNC software.
4. OTHER – There are many other exotic router bit materials available... Diamond, Diamond like, poly crystalline, and more. These bit materials tend to be used in specialty, high volume, and niche markets.

You can find more details on CNC Router Bit Basics

Helical Direction

A CNC router spins a cutter clockwise. The helical direction of the flutes as they wrap around the tool determine if chips are ejected towards the top or bottom of the workpiece. True to their name, upcut mills eject chips towards the top of the workpiece, producing a cleanly cut bottom surface. The downside is possible surface splintering or “tearout” on the top surface as the chips are ejected upwards.
Upcutting bits mounted in a CNC pull chips (and your material) up and away from the table. They are great at clearing out chips from your cuts to avoid overheating your bits. They excel at making cuts all the way through material since they just slightly lift the material and scraps up into the end of the bit. Because of the upcutting action, these bits have a tendency to splinter the top surface of sheet goods like plywood and melamine coated particle board. You also need to be very sure that your material is securely held down to the table so the bit doesn’t lift it from the table and chuck it across the room.
Downcut tools do the opposite, producing a smooth upper surface. They are ideal for pieces that have been previously engraved or v-carved and cannot be flipped to hide tearout. In addition, as downcut mills pack the chips into the cut path, they can be used instead of tabs to hold down a workpiece and keep it from moving. Downcutting bits press chips and material back into the cut and into the table. The downshearing action of these bits do a fantastic job of preserving your material’s top surface. Since the chips are forced down into the cut, these bits should never be used to drill holes. The friction of the bit against the compressed chips is enough to melt plastics and start wood on fire.
A third option called a compression or up-down bit offers some of the benefits of both up and downcut bits. The bit is a standard downcut bit until you get to the tip. The direction of the cut is switched making the tip an upcutter. This means that you can cut through materials like plywood and you will get a clean edge on both sides. The top is shear down, the bottom is pulled up. Compression bits are never to be used to drill holes. Once the bit has been plunged beyond the direction change, the chips have no way to escape and get compressed creating an extreme amount of friction and heat. Compression bits are a little more expensive because of the complicated manufacturing of the cutting edge but they are my goto bit for nearly all of my wood cutting.
You can find more details on Guide to CNC Bits

---

Flutes and Chiploads

Number of Flutes Flutes are the helical grooves that wrap around the sides of the end mill. Each flute has a single tooth with a sharp cutting edge (although there can be more than one) that runs along the edge of the flute. As the tooth cuts into the wood, each flute whisks away a small section or “chip”. The fewer the flutes, the more material that is ejected with each tool rotation. The overall cutting depth should never exceed the length of the flutes on an end mill. If cutting deeper than the length of the flutes, the tops of the flutes will be blocked and chips won’t clear, building up heat and reducing tool life.
Chipload Chipload is the thickness of a machined chip as cut by a specific tool type. This is simply the thickness of a chip which is formed during the machining of material. Chipload is important because the proper size chip will carry away heat, promoting long tool life. When the chip is too small, heat is transferred to the cutting tool causing premature bit failure. Too high of a chipload will cause poor edge finish, and transfer cutting load or thrust to the part, possibly causing it to move. A bit in good condition and running at recommended loads will be at room temperature when a cut is finished.
More flutes create a smoother surface finish, while fewer flutes remove material fastest, but make rougher cuts. Proper chipload is important because chips dissipate heat. Hot cutters can lead to suboptimal results, including burned wood, a poor edge finish and dull tooling.

To summarize:

• More flutes create a smoother surface finish
• Fewer flutes are best at chip clearing, keep heat from building up
• Two or four flute cutters are the most common.
• The direction, size, speed and amount of chips being ejected can also damage the surface of the work piece. We can control how the tooling effects the material through our end mill type selection (upcut, downcut or compression) and speed at which we cut.

There are many tables that help you choose the chipload of the job you want to do, which will be needed to calculate the speed of the router. The image below represents one of the chip load charts available online.


Please note that those represent a specific kind of milling bit. Specific loads for your tools can be obtained from your router bit manufacturer.

---

Speed and Feeds

The speed at which we move a cutter across the material is called the “feed rate”. The rate of rotation is called the “speed” and is controlled by how fast the router or spindle turns the cutting tool. Both feed rate and spindle speed will vary based on the material being cut. A general rule of thumb is that you want to move the tool through the material as fast as possible, without sacrificing surface finish. The longer the tool rotates in any one place, the more heat that builds up. Heat is your enemy and can burn your material or radically decrease the life or your cutting tool. Feed rate vs spindle speed: Spindle speed that is too fast paired with a slow feed rate can result in burning or melting. Spindle speed that is too slow paired with a faster feed rate can result in dulling of the cutting edge, deflection of the end mill and possibility of breaking the end mill. A good strategy when selecting a cutter is to attempt to balance feed rate and spindle speed by performing two passes on the work piece. The first pass, called the roughing pass, can be done by using an end mill that will eject a large number of chips at a high feed rate. The second pass, called the finishing pass, then won’t require as aggressive of a cut and can provide a smoother finish at a high speed.

Chipload refers to the physical size of the chips the bit creates when making a cut. Higher feeedrates produce larger chips. Higher tool rpm produces smaller chips. If your chips are to large, you risk breaking your bit. If your chips are more like a fine powder, you are probably dulling your bit. IT’s a balancing act but start with the manufacturers recommended settings and adjust from there.

Chipload = Feedrate / [RPM x number of flutes]
The nominal surface speeds used for various material are shown in the image below.


Here are some equations you need to know to calculate the spindle speed and the Feed Rate during any job in mind.

1. Spindle Speed

2. Feed Rate
Feed Rate = Spindle Speed (RPM)* Number of Flutes * Chip Load (inches) = Spindle Speed * Number of flutes * Chip Load = Answer inches/min
3. Plunge Rate
Use a plunge rate of 50% or less of the feed rate.

---

Toolpaths

Many settings can change that control the toolpath of the tool. Among those settings are the following:

• Ramp is used to reduce the tool breakage and stress on the material being cut. It occurs by ramping the end mill slowly into lateral cuts, where your tool moves in an XZ or YZ 3D incline into your material to reduce stress on your bit when plunging.