Speeds and feeds calculator.
Spindle RPM and feed rate from surface speed and chip load, in inches and millimeters.
Enter what you know
Every formula this page uses
Every formula here is exact. It is the same geometry a machinist works out on a scrap of paper, so you can check any result by hand.
SFM = (RPM × π × diameter) ÷ 12
Feed rate IPM = RPM × chip load per tooth × number of teeth
Chip load IPT = IPM ÷ (RPM × number of teeth)
Feed per revolution = chip load per tooth × number of teeth
Material removal rate = depth of cut × width of cut × IPM
Metric RPM = (Vc × 1000) ÷ (π × diameter in mm)
Metric feed = RPM × feed per tooth in mm × number of teeth
The twelve in the first expression converts feet to inches. Pi times the diameter is the distance one point on the cutting edge travels per revolution, so dividing surface speed by it gives revolutions. Everything after that is multiplication.
Conventional starting surface speeds, by material
Surface speed depends on much more than the material. The tool, its coating, the rigidity of the setup, the coolant, and the depth of cut all change it, so a table by material can only give you a starting point.
These are the conventional ranges that appear in general machining references. Where the tool manufacturer publishes a figure for the specific cutter, use that figure in place of this table.
Two related numbers come from the same material table. A hole that will be tapped needs a drill size set by the thread engagement you want, which the tap drill sizes page works out. Quoting the job needs the weight of the stock the part is cut from, and weight by material and profile covers bar, hex, tube, plate and rectangle.
| Material | Group | HSS, SFM | Carbide, SFM | Notes |
|---|---|---|---|---|
| Aluminum 6061-T6 | Aluminum | 200 to 300 | 600 to 1200 | The default general purpose alloy. Machines freely and takes anodizing well. |
| Aluminum 7075-T6 | Aluminum | 200 to 300 | 600 to 1000 | Higher strength than 6061 and less corrosion resistant. Common in aerospace. |
| Aluminum 2024-T3 | Aluminum | 180 to 280 | 500 to 900 | |
| Aluminum 5052-H32 | Aluminum | 180 to 280 | 500 to 900 | Sheet alloy. Forms well, which is why it turns up in bend calculations. |
| Aluminum A356 cast | Aluminum | 150 to 250 | 400 to 800 | |
| Steel 1018 (mild) | Steel | 80 to 110 | 300 to 500 | |
| Steel 1045 (medium carbon) | Steel | 70 to 100 | 280 to 450 | |
| Steel 12L14 (free machining) | Steel | 130 to 200 | 400 to 700 | Leaded. Machines faster than any other carbon steel and plates poorly without care. |
| Steel 4140 (alloy) | Steel | 60 to 90 | 250 to 400 | Common shaft and fixture steel. Hardness at delivery changes the numbers substantially. |
| Tool steel A2 | Steel | 40 to 60 | 150 to 250 | |
| Tool steel D2 | Steel | 35 to 55 | 130 to 220 | |
| Gray cast iron | Steel | 50 to 80 | 200 to 400 | |
| Ductile iron | Steel | 45 to 75 | 180 to 350 | |
| Stainless 303 | Stainless | 60 to 90 | 250 to 400 | The free machining austenitic. Preferred for Swiss work where welding is not required. |
| Stainless 304 | Stainless | 40 to 70 | 200 to 350 | Work hardens quickly. A light cut that rubs is worse than a heavier cut that shears. |
| Stainless 316 | Stainless | 40 to 60 | 180 to 300 | |
| Stainless 410 | Stainless | 50 to 80 | 200 to 350 | |
| Stainless 17-4 PH | Stainless | 40 to 60 | 150 to 300 | Numbers move a long way between condition A and the aged conditions. |
| Brass C360 | Copper alloys | 150 to 300 | 400 to 800 | |
| Copper C110 | Copper alloys | 100 to 200 | 300 to 600 | Gummy. Sharp tools and positive rake matter more than speed. |
| Bearing bronze C932 | Copper alloys | 100 to 200 | 300 to 600 | |
| Titanium Ti-6Al-4V | Superalloys | 30 to 50 | 100 to 200 | Low thermal conductivity puts the heat in the tool. Constant feed, no dwelling. |
| Titanium CP grade 2 | Superalloys | 40 to 70 | 150 to 250 | |
| Inconel 718 | Superalloys | 15 to 30 | 60 to 120 | Work hardens severely. Rigidity and a positive depth of cut matter more than surface speed. |
| Inconel 625 | Superalloys | 15 to 30 | 60 to 120 | |
| Monel 400 | Superalloys | 30 to 50 | 100 to 180 | |
| Magnesium AZ31 | Other metals | 300 to 600 | 800 to 1500 | Chips are flammable. Dry machining and swarf handling are safety matters. |
| Nickel 200 | Other metals | not listed | 100 to 200 | |
| Acetal (Delrin) | Plastics | not listed | 500 to 1000 | |
| Nylon 6/6 | Plastics | not listed | 400 to 900 | |
| UHMW polyethylene | Plastics | not listed | 500 to 1000 | |
| PTFE | Plastics | not listed | 300 to 700 | |
| Polycarbonate | Plastics | not listed | 300 to 700 | |
| PEEK | Plastics | not listed | 300 to 600 | |
| ABS | Plastics | not listed | 300 to 700 |
Questions machinists ask about speeds and feeds
How do you calculate RPM from surface feet per minute?
Multiply the surface speed in feet per minute by twelve, then divide by pi times the cutter diameter in inches. RPM = (SFM x 12) / (3.1416 x D). The twelve converts feet to inches, and pi times the diameter is the circumference the cutting edge travels in one revolution. In metric the same relationship is RPM = (Vc x 1000) / (3.1416 x D), with cutting speed in meters per minute and diameter in millimeters.
How do you calculate feed rate from chip load?
Multiply spindle speed by the chip load per tooth and by the number of teeth. IPM = RPM x IPT x number of flutes. The result is inches per minute of table or axis movement. Working backward, chip load is the feed rate divided by the spindle speed and the flute count, and that is the calculation to run when you want to know what a program is actually asking the tool to take.
What surface speed should I use?
Start with the tool manufacturer’s data for the specific cutter, because it accounts for the substrate, the geometry, and the coating in a way no general table can. Where you do not have that, the ranges on this page are the conventional starting points by material and tool type. Begin there, then adjust from what the cut sounds like, what the chips look like, and how the tool wears.
What is material removal rate and why does it matter?
Material removal rate is the volume of material a cut removes per minute, calculated as depth of cut times width of cut times feed rate. It decides cycle time, and it tells you whether the spindle has the power for the cut you have programmed. Two setups with identical speeds and feeds can have very different removal rates, and the one with the higher rate finishes first.
Does chip load change with radial engagement?
Yes, and it is the most common reason a calculated feed rate misbehaves. When radial engagement drops below about half the cutter diameter, the actual chip becomes thinner than the programmed feed per tooth, and the tool rubs instead of cutting. Light radial cuts need a higher feed to make up for it, and that is what chip thinning compensation in a CAM system does.
Is this calculator accurate for turning as well as milling?
Yes, with one adjustment. The speed relationship is identical for turning, with the workpiece diameter in place of the cutter diameter. Turning feed is quoted per revolution instead of per tooth, so set the number of teeth to one and read the chip load figure as inches per revolution.
Who made it, and what it does not do
This tool was written by Shopfloor Agency's lead engineer, who holds a bachelor’s degree in mechanical engineering and builds websites for US manufacturers. It runs entirely in your browser.
The arithmetic is exact. The surface speed table gives conventional starting ranges, because surface speed depends on the tool, the coating, the rigidity of the setup, and the coolant, and this page cannot see any of those. The calculator does not adjust for chip thinning at low radial engagement, for the power available at your spindle, or for what the fixture will tolerate. Use it to get to a starting number quickly, then listen to the cut.
If you spot an error, tell us, and we will correct the page and note the change.
We build websites for the shops that use tools like this.
We work only with US manufacturers and industrial service companies, so you never have to explain your trade. A website is a fixed $6,000, and the source code is yours at launch. Tell us what you make and who buys it, and we will reply with the scope and a delivery date.