What SFM should I use for 6061 aluminum with a carbide end mill?

For 6061-T6 with a coated carbide end mill (TiAlN or AlTiN), start at 800-1500 SFM. Uncoated carbide runs 600-1000 SFM. HSS runs 200-400 SFM. These are starting points for a rigid setup. Reduce if you get chatter or poor finish.

What is chip load and why does it matter?

Chip load is the thickness of material each flute removes per revolution. Too low and you rub instead of cut, generating heat and work-hardening the surface. Too high and you overload the tool. For a typical 0.5 inch 3-flute carbide end mill in aluminum, chip load is 0.005-0.010 inches per tooth.

How do I calculate feed rate for milling?

Feed rate in inches per minute equals chip load times number of flutes times RPM. For example: 0.005 in/tooth chip load, 3 flutes, at 5000 RPM gives 0.005 * 3 * 5000 = 75 IPM feed rate.

What is the difference between SFM for HSS and carbide?

Carbide tools typically run 3 to 5 times faster than HSS because carbide stays hard at much higher temperatures. A coated carbide tool adds another 20-40 percent above uncoated carbide. This is why shops replace HSS with carbide as soon as the job volume justifies it.

How do I machine stainless steel without work hardening?

Keep the tool cutting, never rubbing. Use adequate chip load (at least 0.003 in/tooth for milling), keep SFM in the 200-400 range for coated carbide, and use flood coolant. If you see a glazed surface and the tool starts squealing, the previous pass work-hardened and you need to take a heavier cut to get below the hardened layer.

What is material removal rate (MRR) and how do I calculate it?

MRR is width of cut times depth of cut times feed rate, in cubic inches per minute. It tells you how fast you are removing material. Higher MRR means shorter cycle times but requires more spindle power and machine rigidity. A typical small VMC can sustain 5-15 cubic inches per minute in aluminum.

Free Calculator

Speeds & Feeds Calculator
for CNC Machining

Pick your material, tool coating, and operation. Get recommended SFM, RPM, chip load, feed rate, and material removal rate. Shows the formulas so you know why.

Your setup

Operation

Workpiece material

Tool material / coating

Tool

Tool diameter

in

Number of flutes

Cut parameters (for MRR)

Width of cut (radial)

in

Depth of cut (axial)

in

Recommended RPM

8,785

1,150 SFM (range: 800–1,500)

Feed rate

224.0 IPM

Chip load: 0.0085 in/tooth

Breakdown

Material6061-T6 Aluminum

ToolCarbide (TiAlN)

Diameter0.5 in

Flutes3

SFM (midpoint)1,150

RPM8,785

Chip load (per tooth)0.0085 in

Feed rate224.0 IPM

MRR5.60 in³/min

Formulas used

RPM = SFM × 12 / (π × diameter)

Feed = chip load × flutes × RPM

MRR = WOC × DOC × feed rate

Starting-point recommendations. Always verify against your tool manufacturer's specs, especially for depth of cut and rigidity. Reduce speeds for interrupted cuts, thin walls, and long stick-out.

Next step

Price the job with your cycle time →

Got your feed rate and cutting time? Use the Job Quote Calculator to turn cycle time into a part price.

Reference

Calculate material weight and cost →

Need to estimate material cost for your quote? The Metal Weight Calculator gives you weight and approximate $/lb.

How speeds and feeds work

Every cutting operation has two independent variables: how fast the tool spins (speed, measured in surface feet per minute) and how fast it moves through the material (feed, measured in inches per minute). Get these wrong and you break tools, burn material, or chatter. Get them right and the machine cuts cleanly with good tool life.

Surface speed (SFM)

SFM is the speed at which the cutting edge moves across the workpiece surface. It depends primarily on the workpiece material and the tool material/coating. Harder materials require lower SFM. Better coatings allow higher SFM. The formula to convert SFM to RPM is:

RPM = SFM × 12 / (π × tool diameter in inches)

A smaller tool at the same SFM spins faster. A 1/4" end mill at 500 SFM runs at 7,640 RPM. A 1" end mill at the same SFM runs at 1,910 RPM.

Chip load and feed rate

Chip load is the thickness of material each cutting edge removes per revolution (drilling) or per tooth (milling). It's measured in thousandths of an inch. Too thin and you rub instead of cut, generating heat and work-hardening the surface. Too thick and you overload the tool.

Feed rate (IPM) = chip load × number of flutes × RPM

For drilling, the feed rate is simply chip load per revolution times RPM (one cutting edge, effectively).

Material removal rate (MRR)

MRR tells you how much material you're removing per unit time. For milling:

MRR = width of cut × depth of cut × feed rate

MRR is useful for estimating cycle times and comparing roughing strategies. Higher MRR means faster cycle times but requires more machine rigidity and spindle power.

HSS vs. carbide vs. coated carbide

HSS (high-speed steel) tools are cheap and forgiving but run at much lower speeds. Uncoated carbide typically runs 3–5× faster than HSS. TiAlN and AlTiN coatings add another 20–40% on top of uncoated carbide by reducing friction and heat at the cutting edge. The coating choice matters most in harder materials like stainless and titanium.

When to reduce from the recommended values

The values this calculator shows are starting points for stable, rigid setups. Reduce speed and/or feed for: long tool stick-out (more than 3× diameter), thin-wall parts, interrupted cuts, poor fixturing, older machines with less rigidity, or when chatter appears.

Frequently asked questions

RPM equals SFM times 12 divided by pi times the tool diameter in inches. For example, 500 SFM with a 0.5 inch end mill gives RPM = 500 * 12 / (3.14159 * 0.5) = 3,820 RPM.

Free tool from swarf.shop. No email, no signup, no catch. We build job tracking software for small machine shops — these calculators are stuff we needed ourselves.

Speeds & Feeds Calculatorfor CNC Machining