CNC Router Feeds & Speeds Calculator
Free feed rate, RPM and chip load calculator for CNC routers. Pick your machine class, material, bit and depth per pass. Set a spindle speed or feed rate and the calculator suggests the other, then checks your chip load against the target range for that setup.
Chip Load per Tooth
0.0029 in/tooth
In the target range for this setup. Target 0.0023–0.0035.
- Feed Rate
- 104 IPM
- Spindle Speed
- 18,000 RPM
- Plunge Rate
- 42 IPM
- Depth per Pass
- ≤ 0.125"
Targets come from the same measured data as our Vectric & Fusion tool libraries: a Rigid Hobby machine cutting hardwood with a 2-flute end mill, scaled for your machine class, material, flute count and depth. Every machine is different, so treat these as starting points.
High Country Tools is not responsible for tool breakage. Consider reducing starting feeds by 20% before using the recommended settings from this calculator.
The Feed Rate Formula
Feed rate (IPM) = RPM × flutes × chip load. Chip load is the target; RPM and feed are what you set. Keep the chip load in range and the bit cuts instead of rubbing.
Starting Chip Loads for Hardwood
2-flute end mill, rigid hobby machine (Onefinity, Shapeoko 5 Pro, Altmill and similar), depth ½ × diameter, 18,000 RPM. Measured at 1/4" on our own Onefinity Elite; other sizes follow the same curve. Use the calculator above for other machines and materials.
| Bit diameter | Chip load (in/tooth) | Feed at 18,000 RPM |
|---|---|---|
| 1/16" | 0.0012 | 43 IPM |
| 1/8" | 0.0017 | 61 IPM |
| 3/16" | 0.0023 | 83 IPM |
| 1/4" | 0.0029 | 104 IPM |
| 3/8" | 0.0034 | 122 IPM |
| 1/2" | 0.0039 | 140 IPM |
Starting Settings by Material
1/4" 2-flute end mill, rigid hobby machine, up to 1/8" deep per pass. Each material has its own spindle speed; the feed is spindle speed × 2 flutes × chip load. Change any of it in the calculator above.
| Material | Spindle speed | Chip load (in/tooth) | Feed rate |
|---|---|---|---|
| Hardwood | 18,000 RPM | 0.0029 | 104 IPM |
| Dense Hardwood (maple, oak, ash) | 18,000 RPM | 0.0026 | 94 IPM |
| Softwood (pine, cedar, fir) | 17,000 RPM | 0.0033 | 113 IPM |
| Plywood - Baltic Birch | 18,000 RPM | 0.0028 | 99 IPM |
| Plywood - Melamine / Laminate | 18,000 RPM | 0.0025 | 89 IPM |
| MDF / Particleboard | 17,000 RPM | 0.0032 | 108 IPM |
| Acrylic / PVC (hard plastic) | 12,500 RPM | 0.0036 | 91 IPM |
| HDPE / UHMW / Nylon (soft plastic) | 11,500 RPM | 0.0041 | 93 IPM |
| Epoxy / Resin | 14,500 RPM | 0.0023 | 67 IPM |
| Aluminum 6061 | 16,000 RPM | 0.0016 | 51 IPM |
Starting Feed by Machine Class
1/4" 2-flute end mill in hardwood at 18,000 RPM. Stiffer, more powerful machines can feed faster; pick your class in the calculator.
| Machine class | Examples | Feed rate |
|---|---|---|
| Hobby - Ultralight | Genmitsu, SainSmart, FoxAlien, Small 3018 machines | 47 IPM |
| Hobby - Light | Shapeoko 3 & 4, X-Carve, Longmill, MillRight | 73 IPM |
| Hobby - Rigid | Onefinity, Shapeoko 5 Pro, Altmill, Axiom | 104 IPM |
| Business Class | ShopSabre, AvidCNC, CAMaster | 261 IPM |
| Industrial Class | Onsrud, Biesse, Multicam, Thermwood, SCM | 313 IPM |
Feeds & Speeds FAQ
How do you calculate feed rate for a CNC router?
Feed rate (inches per minute) = spindle RPM × number of flutes × chip load per tooth. A 1/4" 2-flute end mill at 18,000 RPM and 0.0029" chip load runs about 104 IPM.
What is chip load?
Chip load is the thickness of material each cutting edge removes per revolution. Too small and the bit rubs, heats up and dulls; too large and it deflects, chatters or breaks.
How do I know if my feed rate is too slow?
Fine dust instead of chips, burn marks, a squealing sound and a hot bit all mean the chip load is too low. Raise the feed rate or lower the RPM.
How deep should each pass be?
On hobby machines start around half the bit diameter per pass in hardwood. Industry charts reduce chip load about 25% at 2× diameter depth and 50% at 3× diameter. For deep cuts with long bits, an adaptive toolpath with a light stepover is safer.
Does this calculator work for Shapeoko, Onefinity, X-Carve and other hobby machines?
Yes. Pick the machine class that matches your router: Ultralight, Light Hobby (Shapeoko 3 & 4, X-Carve, LongMill) and Rigid Hobby (Onefinity, Shapeoko 5 Pro, Altmill) cover desktop and hobby machines; Business and Industrial cover shop routers and spindles.
What spindle speed (RPM) should I use for different materials?
Our presets run 17,000 to 18,000 RPM in wood and sheet goods, 14,500 in epoxy, 12,500 in acrylic and PVC, 11,500 in HDPE and nylon, and 16,000 in aluminum. Plastics run slower so the chips stay cool instead of melting back into the cut. The tables on this page show the feed rate that goes with each.
Does a longer bit need slower feeds?
Yes. A long cutting length or a lot of bit sticking out of the collet flexes more, so it needs a lighter chip load and a shallower pass. Enter the flute length and stickout in the calculator and it reduces the suggestion for long bits and flags a bit that is long for its size. Choking the bit up in the collet helps.
What is adaptive clearing, and what feed should I use?
Adaptive (high-efficiency) toolpaths cut deep with a light sideways stepover, so only a small slice of the bit is in the material at once. That thins the chip, which allows a faster feed than a normal slot at the same chip load. Pick Adaptive in the calculator's cut type and it suggests the depth, stepover and feed together.
What is the difference between upcut, downcut and compression bits for feeds?
The chip load comes mainly from the bit diameter and the material. The flute direction decides how the chips leave: an upcut clears chips out of deep slots, a downcut pushes them into the cut for a clean top edge so it likes lighter passes in deep pockets, and a compression bit does both for clean edges on plywood and melamine.
Are these exact settings for my machine?
They are starting points. The reference point was measured on our own Onefinity Elite and the other sizes, materials and machine classes follow from it. Start in the lower half of the suggested chip load range, listen to the cut, check the chips, and adjust in 10% steps.
Do you have feeds and speeds for Vectric and Fusion 360?
Yes. Our free tool libraries load these starting values straight into VCarve, Aspire and Fusion 360 for every HCT bit and machine class.
Load these numbers straight into your CAM with the free Vectric & Fusion 360 tool libraries, or find the right bit in the Tool Finder.