Photo via Unsplash
Complete CNC router bit reference for feed rate (IPM), spindle speed (RPM), and depth of cut across 8 materials: softwood, hardwood, plywood, MDF, acrylic, aluminum, HDPE, and foam. Includes chip load formula and bit selection guidance. Updated March 2026.
As an Amazon Associate, we earn from qualifying purchases. See all recommendations
Chip load is the single most important concept in CNC routing. Every feeds and speeds decision flows from it. A correct chip load means efficient cutting, cool temperatures, long bit life, and clean surface finish.
To find feed rate when you know your target chip load:
Feed Rate (IPM) = Chip Load x RPM x Number of Flutes
| Bit Diameter | Material | Target Chip Load | Notes |
|---|---|---|---|
| 1/8" (3.175mm) | Softwood | 0.002–0.004" | Small bit = small chip load |
| 1/8" (3.175mm) | Aluminum | 0.001–0.002" | Use single-flute bit |
| 1/4" (6.35mm) | Softwood | 0.005–0.008" | Most common bit size |
| 1/4" (6.35mm) | Hardwood | 0.004–0.007" | Reduce for harder species |
| 1/4" (6.35mm) | Acrylic | 0.003–0.006" | O-flute or single-flute |
| 1/4" (6.35mm) | Aluminum | 0.001–0.003" | Single-flute, coolant |
| 3/8" (9.525mm) | Softwood | 0.007–0.012" | Larger chip load |
| 1/2" (12.7mm) | Softwood | 0.010–0.018" | High feed rate required |
| 1/2" (12.7mm) | Hardwood | 0.008–0.014" | Reduce for dense woods |
| Problem | Likely Cause | Fix |
|---|---|---|
| Bit burning, discoloration | Chip load too low (rubbing) | Increase feed rate or decrease RPM |
| Bit breaking | Chip load too high | Decrease feed rate or increase RPM |
| Melted material (acrylic, HDPE) | Too much heat, low chip load | Increase feed rate, check flute type |
| Fuzzy edge on wood | Chip load too low or dull bit | Increase feed rate or replace bit |
| Chip re-welding (aluminum) | Chips not clearing, no coolant | Add air blast, reduce depth per pass |
| Chatter marks | Too much depth, deflection | Reduce depth of cut or stepover |
Settings for 2-flute upcut spiral carbide bits unless otherwise noted. Use these as starting points — adjust based on your specific machine's rigidity, spindle power, and workholding.
| Bit Diameter | Flutes | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/8" | 2 | 22,000–24,000 | 60–90 | 1/8" (1x dia) | Light passes, small bit |
| 1/4" | 2 | 18,000–22,000 | 100–150 | 1/4" (1x dia) | Standard production setting |
| 1/4" | 2 | 18,000 | 120–180 | 3/8" (1.5x dia) | Push deeper on rigid machines |
| 3/8" | 2 | 16,000–18,000 | 140–200 | 3/8" (1x dia) | Faster material removal |
| 1/2" | 2 | 14,000–18,000 | 180–250 | 1/2" (1x dia) | High feed required for chip load |
| 1/2" compression | 2 | 16,000–18,000 | 150–220 | Full depth (single pass) | Up/downcut for clean top and bottom |
| Bit Diameter | Flutes | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/8" | 2 | 20,000–22,000 | 40–70 | 1/16" (0.5x dia) | Shallow passes in hard species |
| 1/4" | 2 | 16,000–20,000 | 80–130 | 1/4" (1x dia) | Reduce for very hard woods |
| 3/8" | 2 | 14,000–18,000 | 110–170 | 5/16" (0.8x dia) | More rigidity required |
| 1/2" | 2 | 12,000–16,000 | 140–210 | 3/8" (0.75x dia) | Reduce depth for dense hardwoods |
| Bit Diameter | Bit Type | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/4" | Upcut spiral | 18,000–20,000 | 100–140 | 1/4" | Good chip evacuation |
| 1/4" | Downcut spiral | 18,000–20,000 | 80–120 | 1/8" | Clean top surface, shallow passes |
| 1/4" | Compression | 16,000–18,000 | 100–150 | Full depth | Best surface on both faces |
| 3/8" | Upcut spiral | 16,000–18,000 | 140–190 | 3/8" | Faster for thick sheets |
| 1/2" | Compression | 14,000–18,000 | 150–220 | Full depth | Production nesting operations |
| Bit Diameter | Bit Type | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/4" | Upcut spiral | 18,000–22,000 | 120–180 | 1/4" | MDF cuts easily but dulls bits fast |
| 1/4" | Downcut spiral | 18,000–22,000 | 100–150 | 1/8" | Reduces top-face tearout |
| 3/8" | Upcut spiral | 16,000–20,000 | 160–240 | 3/8" | High feed needed for chip load |
| 1/2" | Upcut spiral | 14,000–18,000 | 180–280 | 1/2" | Cabinet production setting |
MDF is abrasive due to its resin content. Expect 50–70% shorter bit life compared to solid wood. Use carbide bits and consider diamond-coated tools for high-volume production. Always use dust collection — MDF dust is a respiratory hazard.
Acrylic cuts cleanly at high feed rates with single-flute (O-flute) bits. Low chip load causes heat that melts and re-fuses the material. Cast acrylic machines better than extruded acrylic — extruded is more stress-prone and may crack.
| Bit Diameter | Bit Type | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/8" | Single-flute (O-flute) | 18,000–22,000 | 50–80 | 1/16" | Small passes in thin acrylic |
| 1/4" | Single-flute (O-flute) | 16,000–20,000 | 80–130 | 1/8" | Best surface finish |
| 1/4" | 2-flute upcut | 14,000–18,000 | 60–100 | 1/8" | Increase feed to avoid melting |
| 3/8" | Single-flute (O-flute) | 14,000–18,000 | 100–160 | 3/16" | Faster removal, thicker stock |
| 1/2" | 2-flute upcut | 12,000–16,000 | 120–180 | 1/4" | High feed to maintain chip load |
HDPE is soft and gummy — it tends to melt and re-weld if chip load is too low. Single-flute bits and aggressive feed rates are key. HDPE is forgiving of imperfect settings compared to acrylic.
| Bit Diameter | Bit Type | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/4" | Single-flute (O-flute) | 16,000–20,000 | 80–140 | 1/4" | High feed to prevent re-welding |
| 1/4" | 2-flute upcut | 14,000–18,000 | 70–120 | 1/8" | Adequate for most HDPE work |
| 3/8" | Single-flute | 14,000–18,000 | 110–170 | 3/8" | Fast removal of thick stock |
| 1/2" | Single-flute | 12,000–16,000 | 140–200 | 1/2" | High feed rate required |
Aluminum is machinable on hobby CNC routers with correct settings. The biggest risk is heat from chip re-cutting — ensure chips clear the cut zone with compressed air or mist coolant. Never let aluminum chips pile up in the cut.
Use compressed air or cutting fluid to clear chips continuously. Aluminum chips re-welding to the bit cause instant failure. Keep depth of cut shallow (0.010"–0.040" per pass), use carbide single or two-flute end mills, and never use router bits designed for wood on aluminum.
| Bit Diameter | Flutes | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| 1/8" | 1 | 16,000–20,000 | 20–35 | 0.010" | Very shallow, air blast required |
| 1/8" | 2 | 14,000–18,000 | 15–25 | 0.008" | Slower, more careful |
| 1/4" | 1 | 12,000–16,000 | 30–55 | 0.020" | Standard hobby CNC aluminum |
| 1/4" | 2 | 10,000–14,000 | 25–45 | 0.015" | More rigid machines |
| 3/8" | 2 | 10,000–14,000 | 40–70 | 0.025" | Stiff machine required |
| 1/2" | 2 | 8,000–12,000 | 50–80 | 0.030" | Industrial-class CNC machine |
These settings assume a hobby to mid-grade CNC router (Shapeoko, X-Carve, Avid, Onefinity) with standard spindle. Industrial VMCs run 10–20x higher feed rates. Reduce all values by 25% for less rigid machines.
| Foam Type | Bit Type | RPM | Feed Rate (IPM) | Depth per Pass | Notes |
|---|---|---|---|---|---|
| Sign foam (PVC foam board) | O-flute or upcut | 16,000–20,000 | 150–250 | 1/2"–full depth | Very easy to cut, high feed |
| Rigid tooling foam | Ball nose or upcut | 14,000–18,000 | 120–200 | Full depth | 3D carving, prototype work |
| EPS foam (styrofoam) | Any sharp bit | 10,000–16,000 | 200–400 | Full depth | Extremely easy, any sharp bit |
| HDU (high-density urethane) | Upcut or V-bit | 14,000–18,000 | 100–180 | 1/4"–1/2" | Sign carving, clean detail |
Understanding milling direction helps you get better surface finish and extend bit life.
| Method | Chip Thickness | Surface Quality | Machine Requirement | Best Use |
|---|---|---|---|---|
| Conventional milling | Thin to thick | Good, slightly rougher | Any CNC | Roughing passes, slotting |
| Climb milling | Thick to thin | Excellent, smoother | Rigid, low-backlash | Finishing passes, hardwood |
For hobby CNC routers (Shapeoko, X-Carve, Onefinity, etc.), use conventional milling for roughing to avoid pulling the workpiece and chatter. A light final climb-milling pass (0.005"–0.010" depth) dramatically improves surface finish on hardwood and plastic.
Choosing the right bit geometry matters as much as choosing the right speeds and feeds.
| Bit Type | Best Materials | Advantage | Limitation |
|---|---|---|---|
| Upcut spiral | Wood, plywood, MDF, plastics | Excellent chip evacuation, fast cuts | Slightly rough top surface |
| Downcut spiral | Plywood, laminates, veneered panels | Clean top surface, minimal tearout | Chips stay in cut, shallower passes needed |
| Compression (up/down) | Plywood, laminates, MDF | Clean top and bottom edges simultaneously | Must cut at full depth of upcut section |
| O-flute (single-flute) | Acrylic, HDPE, soft plastics, aluminum | Large chip clearance, prevents melting | Lower rigidity at high forces |
| Ball nose | 3D carving, organic shapes | Smooth 3D surfaces, finish passes | Slow, many overlapping passes needed |
| V-bit (60°, 90°, 120°) | Sign lettering, engraving, chamfers | Sharp, detailed profiles | Depth-sensitive to surface flatness |
| Surfacing bit (fly cutter) | Spoilboard, large flat surfaces | Fast, even surface in one pass | Not for profiling or slots |
These are the bits used by professional CNC operators and serious hobbyists for consistent results and long tool life.
As an Amazon Associate, WorkshopCalc earns from qualifying purchases. This helps support our free calculators and reference guides.
Chip load is the thickness of material removed by each cutting edge per revolution. It is calculated as: Feed Rate (IPM) divided by (RPM x Number of Flutes). Correct chip load prevents heat buildup, extends bit life, and produces clean cuts. Too low a chip load causes rubbing instead of cutting, which generates heat and dulls bits very fast. Too high a chip load overloads the bit and causes breakage. Target chip load ranges are 0.001–0.018" depending on material, bit diameter, and number of flutes.
For CNC routing wood with a 1/4" upcut spiral bit, use 18,000–22,000 RPM for softwood and 16,000–20,000 RPM for hardwood, paired with a feed rate of 80–150 IPM. For a 1/2" bit, reduce RPM to 14,000–18,000 RPM and increase feed rate to 180–250 IPM. The key principle is maintaining proper chip load — larger bits need lower RPM and higher feed rates to avoid rubbing and burning.
Yes, most hobby and mid-grade CNC routers can cut aluminum with the right settings. Use a single-flute or two-flute carbide upcut end mill (never a wood router bit), reduce RPM to 10,000–16,000, use very shallow passes (0.010–0.030" depth), run feed rates of 30–60 IPM for a 1/4" bit, and use compressed air or cutting fluid to clear chips continuously. Heat buildup and chip re-welding are the primary failure modes — keep air blasting the cut at all times.
In conventional milling, the cutter rotates against the direction of feed — chips start thin and get thicker. In climb milling, the cutter rotates with the feed direction — chips start thick and get thinner. Climb milling produces better surface finish and less heat but requires a rigid machine with minimal backlash. For hobby CNC routers, use conventional milling for roughing passes (safer, more forgiving) and a light climb-milling final pass (0.005–0.010" depth) for the best surface finish on hardwood and plastics.