CNC / machinist calculator
Feeds and Speeds Calculator
A feeds and speeds calculator that does what the paid apps do, for free and with the math on the page. Pick a material and tool, set the cut, and it returns spindle RPM, a chip-thinning-corrected feed rate, material removal rate, the spindle horsepower and torque the cut demands, and the tool deflection from your stickout. Then it tells you the one thing that actually matters: which limit you hit first, whether that is spindle power, top RPM, or a long thin tool flexing.
Cut
Machine & setup (for the limit checks)
- Feed rate
- —
- Feed note
- —
- Material removal rate
- —
- Required power
- —
- Spindle torque
- —
- Tool deflection
- —
- Stickout ratio
- —
—
Starting values only. See the cutting-data table for the sourced speeds, chip loads and power constants behind each material.
How it works
Speed and feed are two linked decisions. The speed is how fast the cutting edge moves through the material, set as surface feet per minute (SFM) by the material and tool; with the diameter it fixes the spindle RPM. The feed is how fast the tool advances, built from a chip load, the thickness each flute removes per revolution. RPM equals twelve times SFM over pi times diameter, and feed equals RPM times flutes times chip load.
Where this calculator goes past a three-box widget is the chain after those two numbers. When the radial width of cut drops below half the diameter, radial chip thinning makes the real chip thinner than the programmed feed, so the feed must be raised by a thinning factor to keep the chip at the value your tooling expects. That higher feed raises the material removal rate, which sets the spindle power and torque the cut needs through the material's unit power. The cutting force also bends the tool, and that deflection grows with the cube of the stickout and shrinks with the fourth power of the diameter, so a long reach in a small tool flexes badly.
The calculator runs all of those checks against your machine and setup and surfaces the binding constraint, the first limit you run into. That is the number professional tools sell and free tools leave out: not just a feed, but whether the cut is power limited, speed limited, or deflection limited, so you know what to change.
Worked example
A 1/4 in two-flute carbide end mill in 6061 at 800 SFM: RPM = 12 x 800 / (pi x 0.25) = 12,223 RPM, feed = RPM x 2 x 0.002 = 48.9 in/min. Drop the width of cut to 10% of the diameter and chip thinning bumps the programmed feed about 1.67x for the same real chip.
Frequently asked questions
What are feeds and speeds in machining?
Speed is the cutting-edge surface speed (SFM) that sets spindle RPM for a tool diameter, and feed is how fast the tool advances, built from the chip load per flute. Together they decide how a tool cuts.
How do I calculate spindle RPM from surface speed?
Multiply the surface speed in SFM by 12 and divide by pi times the tool diameter in inches. The shop shortcut RPM equals 3.82 times SFM divided by diameter is the same constant rounded off.
What is radial chip thinning and why does it raise the feed?
When the radial width of cut is under half the diameter, each flute's arc is short and the chip comes out thinner than the feed per tooth. You multiply the feed by a thinning factor so the real chip matches the chip load the tool was designed for.
How much spindle horsepower does a cut need?
Multiply the material removal rate in cubic inches per minute by the material's unit power, then divide by the drive efficiency to get motor horsepower. Steel needs about 1 HP per cubic inch per minute; aluminum needs roughly a third of that.
Why does tool stickout matter so much?
Deflection grows with the cube of the stickout, so doubling the stickout multiplies flex by eight, while halving the diameter multiplies it by sixteen. A long reach in a small tool deflects, chatters and leaves a poor finish, so keep the tool as short as the job allows.
What does the binding constraint tell me?
It is the first limit the cut hits: spindle power, top spindle RPM, or tool deflection. Knowing which one is binding tells you what to change, whether to back off feed and depth, drop the speed, or shorten the tool, instead of guessing.
Are these numbers safe to run as-is?
They are conservative starting points compiled from published tool-maker charts, not limits. Your exact tool, coating, holder runout, machine rigidity and coolant all shift the real numbers, so start under these values and climb up once the cut proves stable.
Related calculators
Sources
- Harvey Tool - Speeds and Feeds (free charts)
- Machining Doctor - chip thinning and machining-power formulas
- Harvey Performance - Introduction to High Efficiency Milling
Every formula on this page is shown and sourced. See how we verify.
These calculators are for planning and as a starting point. Recommended speeds and feeds are published starting values that vary with your specific tool, coating, machine rigidity, workholding and coolant. Always start conservative, listen to the cut, and follow your tool maker data sheet.