CNC Feeds and Speeds Master Guide: Calculations, Chip Load, and Material Charts

Why Feeds and Speeds Matter

Feeds and speeds are the most critical parameters in CNC machining. Get them right, and you produce clean parts with excellent surface finish while maximizing tool life. Get them wrong, and you'll burn bits, break end mills, produce fuzzy cuts, and potentially damage your machine. This guide explains the science behind feeds and speeds, provides proven values for common materials, and teaches you how to calculate optimal parameters for any situation.

Understanding the Key Variables

Spindle Speed (RPM)

The rotational speed of the cutting tool, measured in revolutions per minute. Determined primarily by:

• Tool material: Carbide can run 2-3x faster than HSS due to higher heat resistance
• Tool diameter: Larger tools need lower RPM to maintain the same surface speed
• Workpiece material: Hard materials require lower surface speeds
• Machine rigidity: Less rigid machines (hobby CNCs) need conservative speeds to prevent chatter

Feed Rate (IPM or mm/min)

The speed at which the tool moves through the material. Determined by:

• Spindle RPM
• Number of flutes on the tool
• Desired chip load per tooth
• Machine rigidity and power

Chip Load (IPT or mm/tooth)

The amount of material each flute removes per revolution. This is the most important concept in feeds and speeds. Too small a chip load causes rubbing and heat buildup (work hardening in metals). Too large causes tool breakage. The sweet spot produces actual chips, not dust.

Stepover and Stepdown

• Stepover (radial depth of cut): The width of each pass, typically 10-50% of tool diameter. Adaptive clearing uses 5-15% for aggressive constant engagement.
• Stepdown (axial depth of cut): The depth of each pass. Typically 1-2x tool diameter in wood/plastic, 0.5-1x in aluminum, 0.1-0.3x in steel.

The Fundamental Formula

The core relationship you need to understand:

Feed Rate = RPM × Number of Flutes × Chip Load

And to find the required RPM:

RPM = (Surface Speed × 12) ÷ (π × Tool Diameter) [imperial] RPM = (Surface Speed × 1000) ÷ (π × Tool Diameter) [metric]

Where Surface Speed (SFM or m/min) is a material/tool combination constant from reference tables.

Surface Speed Reference Tables

Carbide End Mills

MaterialSurface Speed (SFM)Surface Speed (m/min) Softwood (pine, fir)800-1500240-460 Hardwood (oak, maple, walnut)600-1000180-300 MDF/Particle board800-1200240-365 Acrylic/Plexiglass400-800120-240 Polycarbonate300-50090-150 Hard plastic (delrin/nylon)400-700120-210 Aluminum (6061)800-1400240-425 Aluminum (7075)600-1000180-300 Brass600-1000180-300 Mild steel (1018)200-40060-120 Stainless steel (304)100-25030-75 Tool steel (O1)80-15024-45 Carbon fiber200-40060-120 Fiberglass (FR4)150-30045-90 Foam (EPS/XPS)2000-5000600-1500

HSS End Mills (run at 40-60% of carbide values)

HSS tools cannot handle the heat and wear of carbide speeds. As a general rule, multiply carbide SFM by 0.4-0.6 for HSS equivalents. HSS is acceptable for wood, plastic, and soft metals on hobby machines where you may not have the RPM to reach carbide's full potential anyway.

Chip Load Reference by Material

Material1/8" (3mm) Tool1/4" (6mm) Tool1/2" (12mm) Tool Softwood0.003-0.005" (0.08-0.13mm)0.005-0.009" (0.13-0.23mm)0.009-0.015" (0.23-0.38mm) Hardwood0.002-0.004" (0.05-0.10mm)0.004-0.007" (0.10-0.18mm)0.007-0.012" (0.18-0.30mm) MDF0.003-0.006" (0.08-0.15mm)0.006-0.010" (0.15-0.25mm)0.010-0.018" (0.25-0.46mm) Acrylic0.002-0.004" (0.05-0.10mm)0.004-0.006" (0.10-0.15mm)0.006-0.010" (0.15-0.25mm) Aluminum0.001-0.003" (0.03-0.08mm)0.003-0.005" (0.08-0.13mm)0.005-0.008" (0.13-0.20mm) Mild steel0.0005-0.0015" (0.013-0.04mm)0.0015-0.003" (0.04-0.08mm)0.003-0.005" (0.08-0.13mm) Stainless steel0.0003-0.001" (0.008-0.025mm)0.001-0.002" (0.025-0.05mm)0.002-0.004" (0.05-0.10mm)

Complete Calculation Examples

Example 1: 1/4" Carbide 2-Flute in Oak (Shapeoko/X-Carve class machine)

• Surface speed for hardwood: 700 SFM
• RPM = (700 × 12) ÷ (3.14159 × 0.25) = 10,700 RPM
• Chip load for 1/4" in hardwood: 0.005" (middle of range)
• Feed Rate = 10,700 × 2 × 0.005 = 107 IPM (2716 mm/min)
• Plunge rate: 50% of feed = 53 IPM
• Stepover: 40% of diameter = 0.100"
• Stepdown: 1x diameter = 0.250"

Example 2: 1/8" Carbide 3-Flute in 6061 Aluminum (desktop CNC)

• Surface speed for aluminum: 1000 SFM
• RPM = (1000 × 12) ÷ (3.14159 × 0.125) = 30,560 RPM → capped at 24,000 (spindle limit)
• Chip load for 1/8" in aluminum: 0.002"
• Feed Rate = 24,000 × 3 × 0.002 = 144 IPM (3658 mm/min)
• Plunge rate: 30% of feed = 43 IPM (use ramp entry instead)
• Stepover: 25% of diameter = 0.031" (adaptive clearing)
• Stepdown: 0.5x diameter = 0.063"

Example 3: 1/16" Carbide 2-Flute in Acrylic (detail work)

• Surface speed for acrylic: 600 SFM
• RPM = (600 × 12) ÷ (3.14159 × 0.0625) = 36,670 → capped at 30,000
• Chip load: 0.003"
• Feed Rate = 30,000 × 2 × 0.003 = 180 IPM (4572 mm/min)
• Use single-flute for acrylic if available — it reduces heat buildup
• Stepdown: 0.5x diameter = 0.031"
• Helical/ramp entries required — no plunging into acrylic

Router Bit Speeds (for router-based CNCs like Shapeoko with Makita/Dewalt routers)

Bit DiameterMakita Dial 1 (10k RPM)Makita Dial 3 (17k RPM)Makita Dial 6 (30k RPM) 1/8" straight/v-bitFast feed or shallow cutsGeneral purposeEngraving only 1/4" end millHardwood, aluminumSoftwood, MDFToo fast — causes burning 1/2" surfacing bitBest for facing/surfacingAcceptableDangerous — excessive vibration 60° V-bitDeep V-carvingStandard V-carvingEngraving fine lines

Makita RT0701C dial settings: 1=10k, 2=12k, 3=17k, 4=22k, 5=27k, 6=30k RPM

Special Considerations by Material

Wood

• Upcut bits clear chips from the cut but can lift thin workpieces. Use downcut for finish passes on plywood and veneers.
• Compression bits (upcut tip, downcut body) are ideal for laminated sheet goods.
• Moisture content matters: green wood needs 20-30% slower speeds than kiln-dried.
• Kerf cleaning: if chips pack in the cut, increase feed rate or chip load.

Acrylic and Plastics

• Heat is the enemy. If you see melted material packing on the bit, increase feed rate or use a single-flute bit.
• Never plunge straight down — always use a ramp or helical entry.
• Flood cooling or mist cooling is beneficial for thick cuts (>6mm).
• Cast acrylic machines better than extruded (cleaner edge, less melting).

Aluminum

• Chip evacuation is critical. Use a compressed air blast or mist coolant. Packed chips cause breakage.
• Single-flute or 2-flute end mills work best on machines under 1HP. More flutes struggle to evacuate chips at hobby RPMs.
• Use climb milling whenever possible for better surface finish.
• Rigid workholding is essential. Aluminum work-hardens if you rub instead of cut.
• Start conservative (800 SFM) and increase 10% per successful job until you find the limit.

Steel and Stainless

• Not recommended for most hobby CNC routers — they lack the rigidity and spindle power.
• If you must: use stubby (short flute length) carbide end mills, very conservative speeds (100-200 SFM for stainless), and extremely light depths of cut (0.005-0.010" stepdown with 1/4" tool).
• Flood coolant is almost mandatory for steel to prevent work hardening.
• Expect slow material removal rates. A 1/4" depth pass in aluminum might take 2 minutes; the same in 304 stainless might take 20 minutes.

Carbon Fiber and Composites

• Dust is extremely hazardous — use a full dust collection system and respirator.
• Diamond-coated or solid carbide bits resist the abrasive nature of carbon fiber.
• Downcut or compression bits reduce fraying on the top surface.
• Keep stepdown shallow (0.5-1mm) to prevent delamination.

Signs Your Feeds/Speeds Are Wrong

SymptomCauseFix Loud squealing/chirpingRubbing — chip load too low or RPM too highIncrease feed rate or decrease RPM Bit breaks suddenlyChip load too high or plunge too aggressiveReduce feed rate; use ramp entry instead of plunge Burn marks on wood/plasticToo slow feed or dull bit generating heatIncrease feed rate; replace or sharpen bit Fuzzy/rough cut surfaceDull bit, wrong bit type, or too fast feedUse sharp bit; try compression bit for wood; reduce feed slightly Chatter/vibration marksToo aggressive cut for machine rigidityReduce stepover to 10-20%; use shorter bit (less stickout) Bit melts plastic to flutesHeat buildup — chip load too lowIncrease feed rate significantly; switch to single-flute Excessive tool wearSurface speed too high for materialReduce RPM 20%; verify you're using carbide for metals Workpiece moves during cutInsufficient hold-downAdd more clamps/tabs; use vacuum table; reduce cutting forces

Free Feeds and Speeds Calculators

• 1c3d CNC Feeds & Speeds tool: Our own calculator — spindle RPM, feed rate, plunge rate, and max depth of cut, no external site needed
• Amana Tool Speed/Feed Calculator (web): Simple web-based calculator with material presets
• F&S Wizard (CNCCookbook): Comprehensive calculator with extensive material database
• G-Wizard Calculator: Professional-grade with free trial; best rigidity modeling for hobby machines
• HSMAdvisor: Another professional option with good material libraries
• MakerDAO Calc: Community-built spreadsheet for common hobby CNCs and materials

Bit sizes, stock thickness, and CAD files often mix metric and imperial units — the Unit & Fraction Converter tool handles mm-to-inch conversions including fractional sizes like 1/8" and 1/4" bits.

Recommended Starter Bit Set

A well-chosen set of 6-8 bits handles 90% of hobby projects:

BitUsePrice 1/4" 2-flute upcut carbide end millGeneral purpose roughing/finishing$8-15 1/8" 2-flute upcut carbide end millDetail work, smaller features$6-10 1/4" single-flute O-fluteAluminum, plastics, fast chip clearance$12-18 1/4" downcut 2-fluteWood finish passes, veneer work$10-16 1/4" compressionPlywood, laminated sheet goods$20-35 60° V-bit 1/4" shankV-carving, chamfering, engraving$8-15 90° V-bit 1/4" shankV-carving, sign making$8-15 1" surfacing/facing bitSpoilboard surfacing, large flat areas$18-30 Total starter set$90-154

If a job also involves tapping threaded holes rather than just cutting, the Drill & Tap Reference tool covers correct tap drill and clearance hole sizes for common fasteners.

Pro Tips

• Always start conservative on a new material or setup. Increase speed by 10% per successful test until you find the edge.
• Listen to your machine. A good cut produces a steady humming sound. Squealing = rubbing = heat = bad.
• Shorter tools are more rigid. Use the shortest bit that reaches your cut depth. Every inch of stickout reduces rigidity exponentially.
• Chip color tells the story in metals: Silver chips = perfect. Gold/straw = getting hot. Blue/purple = way too hot, tool damage occurring.
• Use adaptive/toolpath strategies in your CAM software. They maintain constant tool engagement, allowing more aggressive overall parameters with less risk.
• Keep a cutting log: Record material, bit, RPM, feed rate, stepover, stepdown, and results. This personal database is invaluable.