CAD-CAM Feeds and Speeds

1. Determine the Material Type: Different materials require different cutting parameters. The hardness and density of the material play a role in selecting appropriate feeds and speeds.
2. Identify the Router Bit Type: The type of bit (end mill, ball nose, V-bit, etc.) and its material (carbide, HSS, etc.) will influence the cutting parameters. Different bits are designed for different cutting purposes.
3. Choose a Suitable Cutting Speed (SFM): Cutting speed can be measured in surface feet per minute (SFM). It's the speed at which the cutter's teeth engage with the material, including both rotational and directional movement. It's determined by the material being cut and the type of cutter. You'll often find recommended SFM ranges for different materials and bit types.
   Larger bits generally require slower surface speeds (SFM) compared to smaller bits. This is due to the fact that the outer edge of a larger bit is moving faster than the outer edge of a smaller bit even if they both rotate at the same RPM.
   • Hardwoods (e.g. oak, maple, cherry):
     • 1/8" - 1/4" Bits: 1,500 - 4,000 SFM
     • 1/2" - 1" Bits: 400 - 1,200 SFM
     • 1.5" and up: 250 - 600 SFM
   • Softwoods (e.g. pine, cedar, fir): 1,200 - 1600 SFM
   • Plywood: 1200-1500 SFM
   • Brittle Plastics (eg. Acrylic): 300-400 SFM (Acrylic can be brittle, so lower RPMs are often used to prevent chipping and cracking)
   • Phenolic, Delrin: 700-800 SFM
   • Various plastics: 500 - 1,000 SFM
   • Soft foam (purple/blue foam): 1000-2000 SFM
   • Higher Density Foam (Tooling Board): 1000 - 1500 SFM
4. Determine the RPM: Once you have the cutting speed, you can calculate the RPM (revolutions per minute) of the router bit using the formula:
   1. $\text{RPM}=\frac{\text{SFM}\cdot 3.82}{\text{bit diameter}}$. The constant 3.82 is used to convert from SFM to RPM.
5. Calculate the Feed Rate (IPM): The feed rate is how fast the material is moved into the cutter. It's typically measured in inches per minute (IPM). The feed rate depends on the material and the type of cut you're performing (roughing or finishing). A common formula to calculate feed rate is:
   • $\text{Feed Rate (IPM)}=\text{RPM}\cdot \text{Flutes}\cdot \text{Chip Load}$
     Chip load refers to the amount of material removed by each flute per revolution. Chip load recommendations are usually provided by the manufacturer or can be estimated based on the material and bit type. (SEE LINKS TO CHIP LOAD CHARTS)
     • Chip Load settings for Amana Tools Carbide Flat End Mills (2 and 3 flute)
     • Chip Load for Amana Tools Ball Nose Bits
     • Chip Load for Amana Tools Compression Bits
     • Chip load for Amana Tools Insert Face Mill Tool (ours are RC-2254(1.25in), RC-2241 (1.5in), RC-2257 (2.5in))
     • Chip Load for Amana V-bit
   • Chips too big are caused by aggressive cutting, which puts stress on material and driver motors as well as dulls tooling.
   • Chips too small causes dust, burning of material or overheating bits because of friction.
   • Chip load can be defined as Chip Load = Feed Rate (IPM) / (RPM * number of flutes)
6. Step Down: The amount of depth (change in Z per pass) that a tool makes as it cuts in each pass at each level. As the cut depth gets deeper, you should decrease the feed rate. A conservative cut depth is to use 50% of the bit diameter.
7. Step Over: The amount of surface area which a tool is overlapping a previous cut at the same depth level- so a 1/4” Bit with a 50% Step over cuts 1/8 in of new material with each pass.  If the tool is cutting a dado or channel through the material It is effectively stepping over 100% of the tool diameter for examples profile cutting contours or engraving.
8. Lead-Ins, Lead-Outs, Ramps, and Plunges: these speeds modes all require different speeds than cutting.
   • Lead-ins and ramps are transitions from air into a cutting move. This moment of a cut is a sudden shock on the tool. As a result lead-ins should be about 75-100% of cutting feed rate, but the same spindle speed.
   • Ramps slowly remove material in Z to approach a new cutting depth, and should be about 50% of cutting feed rate.
   • Plunges are high force and should be 25% - 33% of the cutting feedrate. These numbers assume HSS tools (high speed steel) a three-fluted end mill - less flutes will require slower speeds. Do not plunge if you are using a Down Cut bit (use ramp or helical entry instead).
9. Adjust Based on Experience: Initial calculations are a good starting point, but they might need to be adjusted based on the machine's rigidity, the material's behavior, and the quality of the cut you're achieving. It's a good practice to start with conservative settings and gradually increase speeds and feeds while monitoring the results.

Flat End Mill Chip Load Charts

Use these as minimum and maximum values. You might find the best results somewhere in between.

Misc

Equation from Fastener Lab article on feeds and speeds

Spindle Speed– the speed in RPM which the tool is spinning. It can be calculated by the following formula:
V is the cutting speed in feet per min (Often this is known,)
D is the diameter of the cutting tool in inches (also known or easily determined)
S is the spindle speed in revolutions per minute.

Tools

• HSM Advisor Feeds and Speeds Calculator
• Fablab Speed and Feeds Calculator