Chip Formation

As the spindle turns a tool, the cutting edge slices into the material, removing a fragment called a chip. The size of the chip is called chip load.

Chips are not just the waste product of machining—they are key to heat dissipation. The act of cutting a chip generates a small amount of frictional heat. Chips absorb this heat, pulling it away from the tool and the workpiece, as they are ejected through the flutes. If this heat were allowed to build up, it could quickly dull tools, leave burn marks on wood, or even start a fire.

Creating chips that dissipate heat quickly while balancing both cut quality and time spent is fundamental to machining. The speed that a machine turns a cutter has an impact on what materials can be cut and what type of tool can be used. Different machine types have different ranges of spindle speed.

Figure 6-1. Chip formation

What Is a Milling Machine?

Mills were invented in the early 1800s. Originally they were large, heavy, rigid, high-precision, motorized (but not computer-controlled) machine tools made to cut very hard materials like metal. The spindle that rotates a rotational cutter capable of lateral cutting called an end mill is stationary, while the material is clamped in a vice to an x-y moving table.¹ Most mill spindles have a speed range of 3,000–7,000 RPM. Anything higher than 7,000 RPM is considered, routing or high-speed machining (see “High-Speed Spindles”).

What Is a Router?

In 1915, Oscar Onsrud and his son Rudy repurposed a jet motor, creating a hand-held spindle that turned much faster than a mill spindle and ran on compressed air—founding Onsrud Machine Works. In order to cut at higher RPM, Onsrud created a new type of cutting tool that could spin at 30,000 RPM, far faster than any end mill at the time could cut. Called router bits, or router cutters, these tools had modified end-mill geometry that could cut wood at high rotational speeds and lateral feeds.

Modern routers are woodworking power tools that use router bits to carve joinery grooves, decorative moldings, engraving, inlays, or simply to cut out parts. This is usually accomplished by tracing a template, sometimes with a bearing-guided router bit. Routers come in many types and sizes and are usually handheld, but can also be mounted in a table—or attached to a machine frame. Some routers are single speed, but most have adjustable, designated, spindle speeds somewhere between 10,000–25,000 RPM, much faster than mill spindles.

For example, a Porter-Cable 7518 3-1/4 HP variable speed router used on some ShopBots can be adjusted to run at any one of five different speeds: 10,000, 13,000, 16,000, 19,000, or 21,000 RPM.

High-Speed Spindles

Some CNC routers have actual router power tools attached, while others have variable high-speed spindles, so-called to differentiate them from traditional mill spindles, which operate at a much lower RPM.

Overall, high-speed spindles (Figure 6-2) are powerful and much quieter than routers. On large-format CNC routers, like the ShopBot PRSstandard and PRSalpha,² high-speed spindles are industrial-quality components with precision bearings that enable them to cut better and last longer than a router. They also have less runout, or rotational wobble, can operate at full torque (twisting force) at lower RPM without bogging down, and have minutely adjustable speeds from around 5,000–25,000 RPM.

Figure 6-2. High-speed spindle on a ShopBot PRSalpha CNC router

Relating Everything to Everything

Feeds, speeds, and chip load are machining’s trinity. They can be defined separately, but when cutting, all three work together simultaneously to produce chips.

When trying to grasp a concept, always look at how it is measured or calculated. That’s the key to understanding exactly what the thing is, what variables are in play, and what relationships are important.

Speed

Spindle speed, measured in revolutions per minute (RPM) is calculated from a combination of specific aspects of cutter geometry, feed rate, and chip load:

Feed Rate

Feed rate is the velocity at which the tool moves laterally through material. Feed rate is measured in distance per time, or inches per minute, and abbreviated IPM³:

Chip Load

Chip load is the amount of material removed by each flute’s tooth as it makes one revolution while being pushed along at a feed rate and spindle speed. Chip load is measured in feed per tooth, or inches per revolution, abbreviated as IPR:

Where to Begin?

The interconnected nature of feeds, speeds, and chip load are obvious from these equations. At first glance, this seems like a “chicken and egg” problem. If all the variables are dependent on one another, where do you begin?

Start with what you know: namely, that you want to cut plywood on a CNC router and that you’ll need a router bit designed for that purpose.

But before you can select a tool, you’ll need to address the following questions:

• What type of CNC router are you using?

• What type of material are you cutting?

• What is the material thickness?

• How are the parts laid out?

• How is the material being held to the machine?

Safety

Routing has some inherent dangers: machines have moving parts, bits can break, and chips and other particles become airborne. It’s best practice to always wear safety goggles and a proper dust mask (if your shop doesn’t have a dust filtration system). Plus, routers are loud when cutting, so wear ear protection. Spinning spindles can catch and pull in anything that hangs loosely on the body, so always remove jewelry, especially necklaces, and tie back long hair and roll up your sleeves.

Screws and Clamps

Mechanical hold-downs are off-the-shelf items like screws and clamps. Screws are the easiest and most common way to secure large sheets to the sacrifice sheet. They don’t take up much space, and they can be driven in flush with the material being cut. As you cut sheets of 4′ × 8′ plywood for the projects in this book, it’s best practice to add a screw at each of the corners and then add additional screws approximately every two feet around the perimeter of the sheet. Carefully place the screws as close to the edge of the material/machine as possible, so you’ll be able to leave a 1″ margin around your cut files and be confident that you won’t hit any screws when machining.

Clamps are very useful when working with smaller size materials, or when you’d prefer not to mar your workpiece with screw holes. However, clamps have one key disadvantage: they protrude above the workpiece. This means that you’ll need to account for them both in your design and the toolpaths you create to avoid hitting the clamp with the machine.

Vacuum Systems

A vacuum system uses suction to secure material to the machine bed, enormously simplifying the cutting process. It eliminates the need to dedicate material to mechanical fasteners and to plan toolpaths around them. Most significantly, it speeds up the process of taking material and parts on and off the machine.

There are two types of vacuum hold-down systems: conventional and universal. Conventional systems are usually specific to a particular task or process and utilize a small machine area, where a universal system utilizes the entire machine bed and is applicable to a broad range of applications. When we mention a vacuum hold-down in this book, we’re talking about a universal system. Although typically more expensive, they are well suited to jobs that make through cuts in sheet goods.

Figure 6-4. Bill Young’s shop with its ShopBot PRS Alpha CNC router and vacuum hold-down system

End Types

End mills for machining wood have two basic end types: those that are able to plunge straight into material, and those with flattened end flutes that must be ramped in.

Standard/Plunge End

These tools are sometimes called fishtail or swallow tail end mills, due to the indentation at the end of the tool. These tools work well for both profile and pocket cutting. For profile cuts, it produces a completely flat edge surface. For pockets, it leaves a clean, 90-degree angle between the side and the bottom, and gives the bottom of the pocket a flat surface (for further details, see “Pockets”).

Finish/Flat End

The fishtail-style plunge end mill can leave toolmark scratches in the bottom of a pocket, which can be eliminated by using a finish or flat end mill (FEM), which must be ramped into the cut due to its much flatter end.

Ball-nose

A ball-nose end mill has helical flutes and a round end, which is best for contour cutting, and is capable of creating topographic smoothness because its ball end makes minimal contact with curved surfaces.

V-Bit

A v-bit has an angled tip that carves a deep v-shaped groove into the material surface. Typically the sharp bottom of a v-bit is aligned with the toolpath, making it ideal for v-carving, or cutting decorative details with a three-dimensional effect without the need for an actual 3D model. V-bits come in a variety of angles and depths, depending upon your desired depth and width of cut.

Engraving

Engraving tools make a shallow cut along a toolpath. They are capable of etching very fine, often decorative, details into a surface.

Flute Types

End mills for machining wood have radial or helical flutes. Radial flutes are straight grooves that are parallel to the tool’s axis, while helical flutes wrap around the tool.

Higher helix angles clear chips away from the cutting edge faster. Straight tooling with radial flutes have a 0° helix angle, while spirals for cutting wood can have a helix angle of up to 35°. In addition to high helix angles, router bits also have steeper rake (tool attack angle) and clearance angles to evacuate the chips much faster than a traditional end mill.

As the tool turns, the direction of the spiral determines which way chips are ejected. The two basic types of helical end mills are upcut and downcut, shown in Figure 6-7.

Figure 6-7. An upcut tool pushes chips up and out, while a downcut tool forces them down into the kerf, as it cuts

Upcut Spiral

This tool’s flutes eject chips upward, out of the gap created between the cut piece and the waste material (kerf). Because the chips are forced up, the material’s top surface can become chipped or frayed (known as tearout), while the bottom face will be cleanly cut.

Although upcut tools are very efficient at dissipating heat and clearing chips, they have some undesirable effects that can make them a poor choice for routing plywood. The upward chip movement pulls the material up from the cutting bed, creating a troublesome lifting effect on lighter, thinner materials. This movement can also pull at small cut parts and long skinny parts. This can be problematic for vacuum holdowns, and you’ll need to use tabs to keep parts in place.

Downcut Spiral

A downcut spiral’s flutes push chips downward, toward the machine bed. When cutting with ¼″ and 1⁄8″ downcut tools, the chips can become compacted in the kerf, which helps to hold the material against the CNC machine bed.

When through-cutting, the downward force created by the chip ejection can cause tearout on the bottom face, while the top face will have a nice finish.

Compression Spiral

A compression tool is a combination of an upcut and downcut spiral. It pulls material up from the bottom of the cut and down from the top of the cut, leaving a good-quality finish on both the top and bottom faces. This seems ideal, but compression tools are expensive, and most are meant to cut in one pass at full depth.

Straight Flute

These radial two flute tools have a zero-degree angle and create a superior finish in natural wood and wood composites. The entire straight flute makes contact with the material when cutting. Chips are not pushed up or down, creating a good edge quality on most materials.

Conventional Cutting

With conventional cutting, the primary cut is made as the tool exits the material. The chip starts out thin and then ends thick. This can cause end-grain splintering in hardwoods, but it works well for composite sheet goods, like plywood.

This scenario is safer on a table or hand-held router, and because hand-held routers paved the way for CNC tools, this cut type is considered to be the “conventional way.”

Climb Cutting

In a climb cut, the chip starts thick and ends thin. This can result in a smoother cut in materials such as hardwood because it eliminates end-grain splintering. However, the forces created can also mar the finsh and push parts around due to the bit trying to “climb” out of the cut. In addition, the forces created can deflect the tool.

Figure 6-8. Climb versus conventional

Feed Direction Strategies

Although we’re recommending a conventional cut for plywood, this isn’t gospel. Machining advice is always specific to the exact materials and tooling you’re using. Plywood varies greatly between brands, types, and even between batches. Sometimes climb cutting may work better than conventional.

The key is to jump in and test your material/tool pairing and settings. Always cut in the direction that gives you the best finish. Cut some test pieces and look at both the part and the scrap/waste material. If the scrap looks better than your cut parts, reverse the feed direction.

You can also try using an onion-skin strategy. This is a machining methodology that utilizes the strengths of both climb and conventional cutting. First, climb-cut the part, but leave a thin “onion skin” layer behind. Then cut the final pass as a conventional cut.⁵

Smooth Ramps

Smooth ramps work well for easing the tool into large parts. Because center-cutting bits have flutes on both the sides and bottom, and three-axis CNCs can move in the x, y, and z axes at the same time, it’s possible to gradually and smoothly move the rotating tool into material at an incline, as shown in Figure 6-9.

Spiral Ramps

This ramp type slowly eases the tool into the material over the full perimeter of a profile toolpath. Spiral ramps are particularly useful for small parts because machining forces can push them around as they are being cut. If the part becomes dislodged from the main workpiece, it will get caught up by the moving tool, resulting in ugly gouge marks in the part, which can also fly off the machine bed. This is bad for safety, your parts, and your end mills, which can break. Spiral ramps also help to maintain vacuum hold because they help to keep parts from lifting.

Figure 6-9. Smoothly ramping into cut

Tabs

Tabs are small, rectangular sections of uncut material, added to profile toolpaths in CAM software, that keep a part joined to the waste material when making through-cuts. Tab length, thickness, and placement are usually user configurable. Also called bridges, tabs are helpful for keeping small parts in place or long, thin parts from vibrating, especially if you don’t have a vacuum hold-down system.

Offset

Pockets cut using the offset method start at the center of the pocket indentation and move in a spiral pattern until the tool reaches the pocket’s outside edge.

Raster

A raster pocket begins at one end, and the tool moves side to side from one end of the pocket to the other, clearing out a recessed area, as shown in Figure 6-11.

When pocketing visible designs or features, rastering with the grain can help hide toolmarks in wood. However, grain direction when pocketing is more relevant when working with hardwood than plywood. With plywood, you’d need to determine what ply your cut depth will reach, and which way the grain is rotated, a tricky proposition.

Stepover

The amount of tool overlap between passes is called the stepover value. The smaller the stepover percentage, the finer the finish due to the increased toolpath overlap. A stepover value of 50.0%, or one-half the diameter of the bit, is usually enough to minimize tool marks and leave a smooth bottom surface.

Troubleshooting

We recommend using the AtFAB project test pieces, introduced in “Test Pieces” and downloadable from the book’s website, to dial in your feeds and speeds. The test pieces are small, and because you’re already using them to fine-tune joinery fit prior to cutting the full-size project file, they’re also perfect for ironing out machine settings.

If your cuts have a rough surface finish or your bit broke halfway through cutting a part, double-check your CAM settings first, especially the number of zeros (speeds) and the decimal points (feeds). Chapter 7 will explain how to import a design file and create toolpaths in a CAM program.

After checking the numbers, or if you’re using the CAM defaults, here are some tips on how to dial in your feeds and speeds using chip load as a guide.

Figure 6-14. AtFab furniture projects machined by Bill Young, assembled and photographed by Gary Rohrbacher

Check Your Chips

After cutting a test piece, take a look at your chips. As shown in Figure 6-13, well-formed chips often have a curl to them. If they look like fine dust, then they’re too small, and your feed rate was too fast.

Feed a Screaming Bit

If the machine emits a loud, high-pitched noise, or scream, as it cuts through the material, it is “hungry”; feed it by increasing the feed rate.

Cool Tool Test

A tool with a feed rate that is too fast will be warm—or even hot—to the touch. After cutting a part, wait for the machine to come to a complete stop. Tools can get hot enough to burn you, so touch the bottom of the spindle first. If the spindle isn’t noticeably hot, touch the tool shank. If the tool is at room temperature, then your feeds and speeds are properly dissipating heat.

Bracketing the Feed Rate

When you’re having trouble dialing in your settings, always adjust your feed rate first. A process that can help is similar to bracketing in photography. Keeping the speed the same, increase the feed rate until the part finish deteriorates; then back off and decrease the speed by around 10%.

Feeding Too Fast

When a feed rate is too fast, the end-mill evacuates chips too quickly. This rapid removal prevents chips from having enough contact with the end-mill to absorb its heat. This reduced contact causes the tool to retain heat and ultimately fail. Decreasing the feed rate slows the speed of the tool along the toolpath. This decrease in feed increases the duration of contact between the end-mill and chips, so the chips adequately absorb heat before they are ejected.

Feeding Too Slow

When the feed rate is too slow, the chip evacuation doesn’t keep up with the chip formation. These chips retain heat, and this buildup of heat, in combination with the forces of feed, will break your bit. Increasing the feed rate will move the end-mill more quickly along the toolpath, so that the rate of evacuation keeps up with the rate of chip formation.

Decrease Cut Depth

Cut depth is another factor that can lead to suboptimal machining. First, double-check your settings, because it’s easy to enter the incorrect numbers or put a decimal point in the wrong place. If your depth of cut is agressive, then dial it back to match your end-mill diameter.

End-Mill Flutes

As the number of cutting edges increases, your feed rate should increase to prevent burning and premature tool dulling. Using more flutes reduces chip load and improves surface finish, if the feed rate remains the same.

Spindle Speed/RPM

You rarely need to adjust your spindle speed. That’s probably around 12,000 RPM when cutting plywood with a ¼″ diameter two flute tool. It’s typical to pick a speed that works for your material and then adjust the feed rate accordingly, using the formulas in “Machining Variables”. However, speed is another variable that you can consider. When the chip load is too large for your tool to handle, decreasing the RPM will reduce the rate of chip formation. Alternatively, you can increase your spindle RPM to allow the tool to form chips more quickly.

In the next chapter, you’ll get hands-on with CAM software, where you’ll be able to import files, define toolpaths, and run machining simulations.