Enjoy 10% off your first order with code FIRST10 — max $500 discount. Start an Instant Quotehello@rivcut.com
Get an Instant Quote
Currently accepting new projects
Calculator

Feeds and Speeds Calculator

Calculate RPM, feed rate, chip load, and material removal rate for CNC milling and turning. Enter your material, tool, and cut parameters — results update in real time.

Cut Parameters

Recommended: 0.003 - 0.005 in/tooth

Results

Spindle Speed
0 RPM
RPM = SFM × 3.82 / diameter
Feed Rate (IPM) 0
Feed Rate (IPR) 0
Chip Load (per tooth) 0
MRR (in³/min) 0
Est. Horsepower 0
SFM Used --
Get This Part Quoted

Starting values only. Adjust based on machine rigidity, tooling, and coolant. Always verify on your machine.

Recommended Starting Values

These are conservative starting values for carbide end mills with flood coolant. Increase by 10-20% for high-performance coated tooling. Decrease by 20-30% for HSS tools.

Material SFM Range Chip Load (1/4") Chip Load (1/2") Notes
Aluminum 6061800 – 1,0000.003 – 0.0050.005 – 0.008Use 2 or 3 flute; aggressive cuts OK
Aluminum 7075600 – 8000.002 – 0.0040.004 – 0.006Harder than 6061; slightly lower SFM
Steel 1018300 – 4000.002 – 0.0040.004 – 0.006Low-carbon; machines easily with carbide
Steel 4140200 – 3000.002 – 0.0030.003 – 0.005Alloy steel; reduce SFM if heat-treated
Stainless 304100 – 1500.001 – 0.0030.002 – 0.004Work-hardens; keep tool cutting, not rubbing
Stainless 31680 – 1200.001 – 0.0020.002 – 0.003Tougher than 304; use AlTiN-coated tools
Titanium Ti-6Al-4V60 – 1000.001 – 0.0020.002 – 0.003High heat; flood coolant mandatory
Brass 360400 – 6000.003 – 0.0050.005 – 0.007Free machining; great surface finish
Delrin (Acetal)500 – 8000.004 – 0.0080.006 – 0.012Plastic; use sharp uncoated tools, low RPM OK
PEEK200 – 4000.002 – 0.0040.004 – 0.006High-temp plastic; keep feeds up to avoid melting
Free Engineering Review

Get Free DFM Feedback on Your Part

Upload your CAD file and our engineers will review your design for machinability, tolerance feasibility, and optimal toolpath strategy.

  • Feature-by-feature machinability check
  • Toolpath and fixturing recommendations
  • Material and tolerance optimization for cost savings
  • Feeds and speeds guidance for your specific geometry
Upload CAD for Free DFM Review Learn About DFM

Accepts STEP, IGES, SolidWorks, Fusion 360 · Response within 24 hours · No obligation

Feeds and Speeds for Aluminum 6061

Aluminum 6061-T6 is the most common CNC machining material. It cuts easily, holds tight tolerances, and produces excellent surface finishes when feeds and speeds are dialed in correctly.

Recommended Starting Parameters

SFM: 800 – 1,000 for carbide end mills. Uncoated carbide is preferred — coatings like TiAlN can actually cause aluminum to stick to the cutting edge. Use 2 or 3 flute end mills for best chip evacuation.

Chip Load (1/4" end mill): 0.003" – 0.005" per tooth. At 900 SFM, a 1/4" 3-flute end mill runs at 13,752 RPM with a feed rate of 124 – 206 IPM. These are aggressive but standard values for modern CNC machines with adequate spindle power.

Depth of Cut Guidelines

For roughing: use 1× to 2× tool diameter depth with 30-50% radial engagement. For finishing: use 0.01" – 0.03" depth with full-width passes. High-speed machining (HSM) strategies work exceptionally well in 6061 — full-depth, light-radial passes at high feed rates produce the best MRR.

Pro tip: If you see built-up edge (BUE) on your tool when cutting aluminum, your SFM is too low. Increase spindle speed. Aluminum cuts cleaner at higher speeds.

Coolant

Flood coolant or high-pressure through-spindle coolant produces the best results. Mist/air blast works for light cuts. Dry machining is possible at conservative feeds but will reduce tool life and surface quality.

Feeds and Speeds for Stainless Steel 304

304 stainless is one of the most challenging common materials to machine. It work-hardens rapidly, generates significant heat, and punishes incorrect feeds and speeds with premature tool failure.

Recommended Starting Parameters

SFM: 100 – 150 for carbide end mills with AlTiN or TiAlN coating. Use 4-flute end mills for stainless — more flutes means lower chip load per tooth while maintaining a reasonable feed rate.

Chip Load (1/4" end mill): 0.001" – 0.003" per tooth. At 125 SFM, a 1/4" 4-flute end mill runs at 1,910 RPM with a feed rate of 7.6 – 22.9 IPM. These numbers are slow compared to aluminum, and that is correct.

Work Hardening Prevention

The single most important rule with 304 stainless: never let the tool rub without cutting. If your chip load is too light, the tool pushes material instead of cutting it. This creates a hardened layer that destroys the next pass. Always maintain a minimum chip load — do not reduce feed rate as a first response to chatter. Instead, reduce depth of cut or radial engagement.

Pro tip: If your 304 stainless parts are coming out harder than the raw stock, your chip load is too low. The material is work-hardening under the tool. Increase feed per tooth or reduce your number of passes.

Coolant and Tool Selection

Flood coolant is mandatory for stainless steel. Through-spindle coolant is even better. Use variable-helix end mills to reduce chatter. Solid carbide with AlTiN coating gives the best tool life. Expect 30-50% of the tool life you get in aluminum.

Need These Feeds Machined?

Upload your CAD file and get instant pricing. We machine aluminum, steel, stainless, titanium, brass, and engineering plastics in-house. Prototypes ship in as few as 3 days.

Get an Instant Quote

No minimums · 100% Made in USA · Never brokered

Frequently Asked Questions

RPM = SFM × 3.82 / tool diameter. SFM is the recommended surface feet per minute for the material. 3.82 is the constant derived from 12 / pi. Tool diameter is in inches. For example, cutting aluminum at 800 SFM with a 0.5" end mill gives 800 × 3.82 / 0.5 = 6,112 RPM.
Feed rate (IPM) = RPM × number of flutes × chip load per tooth. RPM comes from the SFM formula. Chip load is the thickness of material each flute removes per revolution. For example, a 4-flute end mill at 6,000 RPM with 0.003" chip load gives 6,000 × 4 × 0.003 = 72 IPM.
For aluminum 6061 with a 1/4" end mill, use 0.003" to 0.005" chip load per tooth. Smaller tools need smaller chip loads. A 1/8" end mill should use 0.001" to 0.003". Larger tools like 1/2" can handle 0.004" to 0.006". These values assume carbide tooling with flood coolant.
SFM (surface feet per minute) is the speed at which the cutting edge moves across the workpiece surface. It depends on the material being cut. IPM (inches per minute) is the linear feed rate — how fast the tool moves through the part. SFM determines RPM, and RPM combined with chip load and flute count determines IPM.
To avoid tool breakage: reduce chip load if the tool chatters or deflects, check that radial engagement is not too high for the tool diameter, use the correct SFM for the material, ensure proper coolant coverage, and avoid plunging directly into hard materials. Small tools (under 1/8") are especially fragile — reduce feed rate and depth of cut.
For 304 stainless steel, use 100-150 SFM with carbide tooling. Chip load for a 1/4" end mill is 0.001" to 0.003" per tooth. Use a 4-flute end mill with flood coolant. Keep the tool engaged — do not let it rub without cutting, as stainless steel work-hardens quickly. Reduce SFM by 20% for 316 stainless.
Chip thinning happens when radial engagement (width of cut) is less than 50% of the tool diameter. The actual chip thickness becomes smaller than the programmed chip load, so you need to increase feed rate to maintain the correct chip thickness. Ignoring chip thinning leads to rubbing, heat buildup, and shorter tool life.
Deeper cuts remove more material per pass, reducing the number of passes needed. But deeper cuts also increase cutting force and deflection. A common strategy is to use full flute length depth with light radial engagement (high-speed machining), or shallow depth with full-width cuts. The material removal rate depends on the combination of depth, width, and feed rate.
Material removal rate (MRR) is calculated as width of cut × depth of cut × feed rate (IPM), measured in cubic inches per minute. MRR tells you how productive your machining operation is. Higher MRR means faster cycle times and lower cost per part. But pushing MRR too high causes tool wear, chatter, and poor surface finish. The goal is to find the highest MRR that still produces good parts.
Explore

More Resources

Tap Drill Size Chart | UNC, UNF & Metric Sizes CNC Material Selection Guide Tolerance Fit Chart | Clearance, Transition & Press Fit Press Fit Calculator | Interference Fit Stress & Force Drill Bit Size Chart | Number, Letter & Fractional Threading Standards Guide | UNC, UNF, Metric & NPT CNC Design Guide | Rules for Machinable Parts Surface Finish Chart | Ra, Rz & Process Guide

Related Resources

Calculator

Cutting Speed Calculator

Calculate SFM and RPM for milling and turning operations.

Use Calculator
Calculator

CNC Cost Calculator

Estimate machining cost per part with detailed breakdown.

Use Calculator
Calculator

Material Cost Comparison

Compare CNC machining cost across 9 materials side by side.

Use Calculator
Ready to Start?

Get Exact Pricing for Your Parts

Upload your CAD file and get instant AI pricing. Prototypes ship in as few as 3 days. No minimums required.

Get an Instant Quote Email Us

No minimums · 100% Made in USA · Never brokered · Ships anywhere in the US

Ready to machine your part?

Upload CAD for Instant Quote