CNC Router Feeds and Speeds Calculator

A 1/4" two-flute bit in hardwood on a Shapeoko-class router typically runs about 17,000 to 18,000 rpm at 2,000 to 2,200 mm/min (80 to 85 in/min), 3 mm deep per pass. Pick your machine, material and bit for a starting point that respects your router's speed and feed limits. For metal-cutting mills and lathes use the machine shop speeds and feeds calculator instead. Published November 1, 2026.

Your machine

Picking a machine fills in its usual class, spindle and a typical cutting feed. Defaults are typical, not maker specifications. Change them to suit your machine: the max cut feed is the fastest it cuts cleanly, not its rapid speed.

Material and bit

Check my current settings

Uses the flutes, bit, material and machine above. Leave blank to skip.

Starting Feeds and Speeds

    Your Settings Checked

    Enter your rpm and feed under "Check my current settings" to see the chip load each tooth is taking.

    Router Dial (approximate)

    DialApprox. rpmFeed at this rpm (mm/min)

    Dial speeds are approximate no-load figures and vary between routers; under load they drop. The feed column uses the target chip load and your flutes, so you can pick a different dial and still keep a sensible chip. Rows above your max cut feed are marked.

    How the CNC Router Feeds and Speeds Calculator Works

    On a router the thing that matters most is chip load: how thick a sliver each cutting edge takes per turn. Too thin and the bit rubs, heats up and burns wood or melts plastic. Too thick and a small bit snaps or a light machine loses steps.

    Hobby routers spin fast (10,000 to 30,000 rpm) but cannot feed as fast as an industrial machine, so the usual trap is a feed that is too slow for the spindle speed. This tool starts from a typical chip load for your material, scales it for the bit and machine, then picks the spindle speed and feed that keep that chip within your machine's limits. Every figure here is a rule of thumb gathered from common hobby practice, not tool-maker data. The machine shop speeds and feeds calculator is the one to use for steel and other metals on a milling machine, where cutting speed in metres or feet per minute is the starting point instead.

    The Method

    1. Target chip load (rule of thumb)
    cl = base × clamp(D ÷ 6.35, 0.4, 1.6) × class
    Base chip load in mm/tooth for a 1/4" (6.35 mm) 2-flute carbide bit on a hobby machine: softwood 0.07, hardwood 0.06, MDF 0.08, plywood 0.065, cast acrylic 0.06, HDPE 0.08, PVC foam 0.08, aluminium 0.025, brass 0.02. Class factor: light 0.6, hobby 1.0, rigid 1.5, steel frame / pro 1.8. If the result is under the rubbing minimum (wood 0.025, plastics 0.03, metals 0.01) it is raised to that minimum.
    2. Spindle speed and feed
    feed (mm/min) = rpm × flutes × cl
    in/min = mm/min ÷ 25.4
    Start at about 18,000 rpm for wood, 16,000 for plastics, 12,000 for aluminium and 10,000 for brass, kept inside your machine's range (and snapped to the nearest speed-dial setting if your router has one). If the feed comes out above your max cut feed, the rpm is lowered to keep the chip. If even the lowest rpm is too fast, the feed is capped and you are warned that the chip is thinner than it should be.
    3. Depth, stepover and plunge
    Depth per pass as a multiple of the diameter (light / hobby / rigid / pro): wood, MDF and ply 0.25 / 0.5 / 1.0 / 1.5; plastics 0.25 / 0.4 / 0.6 / 0.8; aluminium and brass slotting 0.05 / 0.1 / 0.2 / 0.3. Pocketing stepover 40 % (25 % in metals). Adaptive clearing 10 to 25 % stepover; on a rigid or steel-frame machine aluminium adaptive can go 1 to 2 × D deep at 10 to 20 %. Plunge about one third of the feed; ramp in at 2 to 3° in aluminium.
    4. Removal rate and checking your settings
    MRR (cm³/min) = depth × width × feed ÷ 1000
    your chip load = feed ÷ (rpm × flutes)
    Your chip load is compared with the target: under the minimum is rubbing, under 75 % is light, 75 to 130 % is good, up to 200 % is heavy, beyond that is too heavy.

    Machine and Spindle Presets

    The machine list sets a class, the spindle the machine usually carries and a typical cutting feed. The class matters most: it reflects how stiff the frame and drives are, which decides how big a chip and how deep a pass the machine can hold without chatter or lost steps.

    ClassTypical machinesUsual spindle
    Light3018, 3020 and 4040-style desktop machines775 DC motor or 300–500 W ER11 spindle
    HobbyOoznest WorkBee, OpenBuilds LEAD, Shapeoko 3 / XXL / 4 / Pro, X-CarveMakita RT0701C / RT0700C, Carbide 3D Compact Router, DeWalt DWP611, or a 0.8–1.5 kW VFD spindle
    Rigid hobbyOnefinity, Shapeoko 5 Pro, Avid Benchtop ProTrim router or 1.5–2.2 kW VFD spindle
    Steel frame / proPrintNC and other steel-frame builds, full-size Avid PRO2.2 kW+ VFD spindle

    Upgrades change the class: a WorkBee or LEAD with stiffer gantry plates and a spindle may cut like a rigid machine, and a worn or loose machine like a lighter one. Only the Makita dial table is a published one; the dial numbers for other routers are estimated as even steps across their speed range, so set by rpm where you can. A VFD spindle is set directly in rpm.

    Worked Example

    1/4" 2-flute upcut in hardwood, hobby machine (Shapeoko-class) with a Makita RT0701C, max cut feed 2,500 mm/min
    • Chip load: 0.06 × (6.35 ÷ 6.35 = 1.0) × 1.0 = 0.060 mm/tooth (0.0024 in), above the 0.025 mm wood minimum.
    • Spindle speed: wood target 18,000 rpm is inside 10,000 to 30,000. The nearest Makita dial is 3 (about 17,000 rpm): 1,000 rpm away, against 4,000 rpm for dial 4.
    • Feed: 17,000 × 2 × 0.060 = 2,040 mm/min, or 2,040 ÷ 25.4 = 80.3 in/min. That is under the 2,500 mm/min limit, so no change.
    • Depth per pass: 0.5 × 6.35 = 3.2 mm. Pocket stepover: 40 % of 6.35 = 2.5 mm. Plunge: 2,040 ÷ 3 = 680 mm/min.
    • Slotting removal rate: 3.175 × 6.35 × 2,040 ÷ 1000 = 41 cm³/min.
    • Without the Makita preset the tool keeps 18,000 rpm and gives 18,000 × 2 × 0.06 = 2,160 mm/min.

    Reading the Chips

    What you see or hearLikely causeWhat to try
    Fine dust, scorch marks, a hot bitChip too thin: feed too slow or rpm too highRaise the feed or drop the rpm (a dial lower on a Makita)
    Small, even chips and a steady humAbout rightKeep it, then try 10 % more feed on the next test cut
    Melted strings or re-welded chips in plasticRubbing and heat, chips not leaving the cutSingle-flute bit, lower rpm, more feed, air blast
    Chatter, screaming, wavy wallsCut too deep or wide for the machine, or a long stick-outShallower passes, shorter stick-out, check belts and V-wheels
    Router bogs down, lost steps, snapped bitChip too heavy or chips packing in the slotLower the feed, shallower passes, better extraction, upcut bit

    CNC Router Feeds and Speeds Chart

    Starting points from this calculator for a hobby-class machine (Shapeoko, WorkBee, X-Carve, OpenBuilds LEAD and similar) with a trim router that runs 10,000 to 30,000 rpm and a 2,500 mm/min cutting feed limit, using carbide upcut bits (single-flute O-flute where listed). Light 3018-style machines need about 60 % of these feeds and half the depth; rigid machines can go higher. Pick your own machine above for numbers that suit it.

    MaterialBitrpmFeed (mm/min)Chip load (mm/tooth)Depth per pass
    Softwood (pine, spruce)1/8" 2-flute18,0001,260 (50 in/min)0.0351.6 mm
    Softwood (pine, spruce)1/4" 2-flute17,8572,500 (98 in/min)0.073.2 mm
    Softwood (pine, spruce)6 mm 2-flute18,0002,381 (94 in/min)0.0663 mm
    Hardwood (oak, maple, walnut)1/8" 2-flute18,0001,080 (43 in/min)0.031.6 mm
    Hardwood (oak, maple, walnut)1/4" 2-flute18,0002,160 (85 in/min)0.063.2 mm
    Hardwood (oak, maple, walnut)6 mm 2-flute18,0002,041 (80 in/min)0.0573 mm
    MDF1/8" 2-flute18,0001,440 (57 in/min)0.041.6 mm
    MDF1/4" 2-flute15,6252,500 (98 in/min)0.083.2 mm
    MDF6 mm 2-flute16,5362,500 (98 in/min)0.0763 mm
    Plywood / birch ply1/8" 2-flute18,0001,170 (46 in/min)0.0331.6 mm
    Plywood / birch ply1/4" 2-flute18,0002,340 (92 in/min)0.0653.2 mm
    Plywood / birch ply6 mm 2-flute18,0002,211 (87 in/min)0.0613 mm
    Cast acrylic (PMMA)1/8" 2-flute16,000960 (38 in/min)0.031.3 mm
    Cast acrylic (PMMA)1/4" 2-flute16,0001,920 (76 in/min)0.062.5 mm
    Cast acrylic (PMMA)6 mm 2-flute16,0001,814 (71 in/min)0.0572.4 mm
    Cast acrylic (PMMA)1/8" 1-flute16,000480 (19 in/min)0.031.3 mm
    HDPE / UHMW1/8" 2-flute16,0001,280 (50 in/min)0.041.3 mm
    HDPE / UHMW1/4" 2-flute15,6252,500 (98 in/min)0.082.5 mm
    HDPE / UHMW6 mm 2-flute16,0002,419 (95 in/min)0.0762.4 mm
    HDPE / UHMW1/8" 1-flute16,000640 (25 in/min)0.041.3 mm
    Aluminium 60611/8" 2-flute12,000300 (12 in/min)0.0130.3 mm
    Aluminium 60611/4" 2-flute12,000600 (24 in/min)0.0250.6 mm
    Aluminium 60616 mm 2-flute12,000567 (22 in/min)0.0240.6 mm
    Aluminium 60611/8" 1-flute12,000150 (6 in/min)0.0130.3 mm

    Rules of thumb, not tool-maker data. Where the feed sits at 2,500 mm/min the spindle speed has been lowered to keep a proper chip; on a Makita, set the nearest dial. Start with a test cut in scrap and listen to the cut.

    Practical Tips

    • Make a test cut and listen. Cut a short slot in scrap with the suggested numbers, look at the chips and listen to the router, then adjust in 10 % steps. Most G-code senders let you override feed while it runs.
    • Upcut, downcut or compression for ply. Upcut clears chips best but lifts fibres on the top face; downcut gives a clean top but packs chips; a compression bit leaves both faces of plywood clean once the first pass is deeper than its upcut tip.
    • Single flute for acrylic and aluminium. One big flute leaves room for chips, so they carry heat away instead of melting or welding. Use an air blast (or a mist) on aluminium and keep chips out of the slot.
    • Hold it down and suck it up. Clamps, screws or tabs stop parts flying when they are cut free. Good dust extraction stops the bit re-cutting its own chips, which is a common cause of burning.
    • Safety. Wear eye and ear protection, and a dust mask for MDF. Never leave a router running unattended: fine MDF and wood dust plus a dull bit or a rubbing cut can start a fire in the dust collector. Keep hands clear while it moves.
    • Small bits, hard metals. For a 1/8" bit or smaller, or for side milling at a light stepover, look at the chip thinning calculator: a narrow cut thins the chip, so the feed can go up.

    More CNC Cutting Tools

    Frequently Asked Questions

    With a 1/4 inch 2-flute bit on a Shapeoko-class machine, a typical start is about 12,000 to 16,000 rpm at 1,900 to 2,500 mm/min (75 to 100 in/min) and about 3 mm deep per pass. That is roughly 0.08 mm per tooth. MDF tolerates heavy chips well; slow feeds are what make it burn.

    Most 3018 spindles top out near 10,000 rpm and the frame is light, so keep cuts small. With a 1/8 inch 2-flute bit in wood try about 10,000 rpm at 500 mm/min (20 in/min) and 0.5 to 1 mm deep per pass. Raise the feed in small steps while the chips stay clean and the machine does not chatter.

    For a 1/4 inch 2-flute bit in hardwood, dial 3 (about 17,000 rpm) at about 2,000 mm/min is a sensible start. Aluminium usually runs on dial 1 or 2 with a single-flute bit, because a hobby machine cannot feed fast enough for higher speeds. The dial speeds are approximate and drop under load.

    Usually the chip is too thin: the feed is too slow for the spindle speed, so the edge rubs instead of cutting. Raise the feed or lower the rpm, clear chips with better dust extraction, and replace a dull bit. Pauses in the toolpath and slow finishing passes also leave burn marks.

    A downcut gives a clean top face for shallow work like inlays and engraving. An upcut clears chips best for deep cuts but can splinter the top veneer. A compression bit gives clean top and bottom faces on through-cuts, as long as the first pass is deeper than its upcut tip.

    A WorkBee with a Makita RT0700C or RT0701C is a hobby-class machine. For a 1/4 inch 2-flute upcut in hardwood, start at dial 3 (about 17,000 rpm) and about 2,000 mm/min, 3 mm deep per pass. In MDF and softwood you can feed a little faster; in aluminium use a single-flute bit, a low dial and shallow passes.

    For a 1/4 inch 2-flute carbide bit on a hobby machine, a typical start is about 0.06 mm per tooth (0.0024 in) in hardwood, 0.07 mm in softwood and 0.08 mm in MDF. Light 3018-style machines need about 60 % of that and rigid machines can take about 1.5 times as much. Below about 0.025 mm per tooth the bit rubs and burns the wood.

    All chip loads, speeds and depths are rules of thumb for carbide router bits, not data for your machine or tooling. Check the bit maker's figures, start with a test cut in scrap, and wear eye and ear protection.