Most machinists learn speeds and feeds the hard way: a broken endmill, a screaming cutter, or a part that looks like it was chewed on by a beaver. The charts in the Machinery's Handbook are a good starting point, but they assume ideal rigidity, perfect coolant delivery, and brand-new tooling. Real shops have worn spindles, long stickout, and that one vise that never clamps square.
The two numbers that matter are surface speed and chip load. Surface speed (SFM) is how fast the cutting edge moves across the work. Chip load is how thick each chip is. Get the surface speed wrong and you burn tools or waste time. Get the chip load wrong and you break tools or leave a garbage finish. This guide covers both, explains how material and coating change the picture, and gives you a framework for dialing in any job without guessing.
Surface Feet Per Minute: The Speed That Actually Matters
RPM is not speed. RPM is how fast the spindle turns. A half-inch endmill at 5,000 RPM is moving at 654 SFM. A one-inch endmill at 5,000 RPM is moving at 1,309 SFM. Same RPM, double the surface speed. That is why you cannot just copy RPM from one job to the next. You have to convert to SFM first, then calculate the RPM for your specific cutter diameter.
The formula is: RPM = (SFM × 3.82) / D, where D is the cutter diameter in inches. SFM targets come from the workpiece material and the tool material. Mild steel with an uncoated HSS endmill runs at 60 to 100 SFM. The same steel with a coated carbide endmill runs at 300 to 600 SFM. Aluminum with carbide can hit 800 to 1,500 SFM or higher. Stainless 304 drops to 200 to 350 SFM because it work-hardens if you rub instead of cut.
The single biggest mistake in speed selection is running too slow in stainless and other work-hardening alloys. Machinists hear "stainless is hard to machine" and cut the speed in half. The tool then rubs instead of shearing, the surface work-hardens into a shell harder than the base material, and the next pass is cutting hardened steel with a feed rate set for soft steel. The fix is to maintain adequate surface speed and chip load so every tooth takes a real chip.
RPM = (SFM × 3.82) / D
D = cutter diameter (inches)
SFM = surface feet per minute
Example: 400 SFM with a 0.500" endmill
RPM = (400 × 3.82) / 0.5 = 3,056 RPM
Speeds & Feeds Calculator
Calculate optimal RPM and feed rate for milling and drilling operations. Select material and tool diameter to get recommended cutting speeds, chip load, and material removal rate with risk tier classification.
Chip Load: Why Feed Matters More Than Speed
Chip load is the thickness of material each cutting edge removes per revolution. For milling: chip load = feed rate / (RPM × number of flutes). For a 4-flute endmill at 3,000 RPM and 24 IPM feed: chip load = 24 / (3,000 × 4) = 0.002 inches per tooth.
Chip load is the single most important variable in tool life. Too thin a chip and the cutting edge rubs instead of shearing. Rubbing generates friction heat without removing material, and that heat goes straight into the tool. The coating breaks down, the substrate softens, and the edge rounds over. You get 15 minutes of tool life instead of 2 hours. Too thick a chip and the cutting forces exceed what the tool can handle. The edge chips, or the tool deflects and leaves a bad finish, or the whole thing snaps.
The sweet spot for most carbide endmills in steel is 0.001 to 0.005 inches per tooth, depending on cutter diameter. A good rule of thumb is chip load equals roughly 1% of the cutter diameter for carbide in steel. A 0.500" endmill targets 0.005" per tooth. A 0.250" endmill targets 0.0025" per tooth.
When you are troubleshooting a cutting problem, check chip load first. If the chips are dust or powder, the chip load is way too low. If the chips are thick, curled, and blue, you are pushing hard but the tool can probably handle it. If the chips are inconsistent in size, you likely have a runout or rigidity problem, not a feeds-and-speeds problem.
Material Groups: Not All Steel Is the Same
Mild steel (1018, A36) is soft and gummy. It wants moderate speed and aggressive chip load to prevent built-up edge. Medium carbon steel (1045, 4140 pre-hard) is tougher and generates more heat. Hardened steel (4140 HRC 40+, D2, H13) requires low speed, rigid setups, and specialized coatings.
Stainless steels split into two camps. Austenitic grades (304, 316) work-harden aggressively and need steady, positive chip loads with no dwelling or rubbing. Martensitic grades (410, 17-4 PH) behave more like medium carbon steel and are generally easier to machine. The key with all stainless is to never let the tool rub.
Aluminum is the opposite problem. It is soft, has a low melting point, and loves to weld itself to the cutting edge. High speed, high chip load, and sharp tools with polished flutes are the solution. Uncoated carbide or ZrN-coated tools work better than TiAlN in aluminum because TiAlN has aluminum in the coating and creates a chemical affinity with the workpiece. Two or three flutes are preferred over four because the wider flute gullets clear chips faster.
Cast iron produces short, broken chips because the graphite in the matrix acts as a chip breaker. Speeds can be surprisingly high (300 to 500 SFM with carbide), but the abrasive graphite and sand inclusions eat uncoated tools quickly. Use coated inserts.
Coated vs Uncoated: When the Coating Earns Its Money
Tool coatings are thin ceramic layers deposited on the carbide substrate. The most common coatings are TiN (gold color), TiCN (blue-gray), TiAlN (dark purple), and AlTiN (black). Each has a temperature range where it performs best.
TiN is the basic coating. It works well in mild steel and general-purpose cutting. It breaks down above about 1,100°F. TiAlN and AlTiN are designed for high-speed dry machining. The aluminum in the coating forms an aluminum oxide layer at high temperatures that actually improves lubricity. These coatings perform worse at low speeds and with flood coolant because they never reach their operating temperature.
If you run flood coolant and moderate speeds, TiN or TiCN is your best bet. If you run dry or with mist at high speed, TiAlN or AlTiN will outlast everything else. If you cut aluminum, use uncoated polished carbide or ZrN, which resists built-up edge without the aluminum-affinity problem of TiAlN.
Coated tools cost 20 to 40 percent more than uncoated. The payback is in tool life: a properly matched coating typically doubles or triples edge life. The mistake is buying coated tools and then running them at uncoated speeds. If you paid for TiAlN, run it at TiAlN speeds or you are wasting the coating.
Flood coolant, moderate speed → TiN or TiCN
Dry or mist, high speed → TiAlN or AlTiN
Aluminum → Uncoated polished or ZrN
Stainless → TiAlN at proper SFM
Cast iron → TiCN or AlTiN
Speeds & Feeds Calculator
Calculate optimal RPM and feed rate for milling and drilling operations. Select material and tool diameter to get recommended cutting speeds, chip load, and material removal rate with risk tier classification.
Dialing It In: A Practical Process
Start with the recommended SFM for your material and tool combination. Calculate RPM from the cutter diameter. Set chip load at the midpoint of the manufacturer's recommendation. Calculate feed rate from RPM, chip load, and flute count. Run the first pass and listen. A smooth, consistent hum is good. Chatter or squeal means something is wrong with rigidity, stickout, or workholding before you blame the feeds and speeds.
If the tool is performing well but you want to push it, increase feed rate first, not speed. Higher feed rate means thicker chips, which carry more heat away from the cut. Higher speed means more heat generated at the cutting edge. Feed is your friend; speed is your limit.
Document what works. Keep a notebook or spreadsheet of material, cutter, coating, SFM, chip load, and tool life for every job. After six months, you will have a reference that is more valuable than any chart because it is calibrated to your specific machines and tooling brands.