Feeds and Speeds

Feeds and speeds are the two groups of cutting parameters that set how a cutting tool removes material: speed — how fast the cutting edge moves through the workpiece — and feed — how fast the tool advances. On a CNC machine both are numbers in a part program, repeated exactly on every part. Set them right and the tool cuts cleanly and lasts; set them wrong and the job crawls or ends in a broken tool and a scrap part. This entry explains what each parameter is, how they work together, and where the starting numbers come from.

What “speed” means on a machine tool

Machinists use two different speeds, and confusing them causes many bad cuts.

Cutting speed — often called surface speed — is how fast the cutting edge travels across the workpiece surface, in metres per minute (m/min). It depends on the two materials meeting at the cut, plus the tool’s coating: carbide cuts a given material far faster than high-speed steel, and a hard alloy far more slowly than aluminium. Cutting speed does not depend on tool size.

Spindle speed is how fast the spindle rotates — in turning, how fast the workpiece rotates — in revolutions per minute (rpm). It exists only to deliver the cutting speed you want at the diameter being cut:

cutting speed (m/min) = π × cutting diameter (mm) × rpm ÷ 1000

usually rearranged to find the rpm: rpm ≈ 318 × cutting speed ÷ cutting diameter. Note the division by diameter: to hold the same cutting speed, a 3 mm end mill spins about ten times faster than a 30 mm face mill — which is why a machine’s maximum spindle speed often caps small-diameter cutters.

In turning the diameter changes as the tool moves across the bar, so the effective cutting diameter is never constant. A CNC lathe running constant surface speed raises the rpm as the diameter shrinks, keeping the cutting speed steady; a fixed-rpm cut runs too hot at the large diameter and too slow at the small.

What “feed” means

Feed is how fast the tool advances through the work. On a mill the whole cutter moves, so feed is a linear rate in millimetres per minute (mm/min); on a lathe the tool advances a set amount per workpiece revolution, so feed is in millimetres per revolution (mm/rev). Drilling is usually programmed per revolution too.

The number that matters most for tool stress and finish is the feed per tooth — in milling, the thickness each cutting edge removes in one revolution, often called the chip load. The linear feed rate is just that figure multiplied across the tool:

feed (mm/min) = rpm × feed per tooth (mm) × number of flutes

A four-flute end mill at 10,000 rpm taking 0.05 mm per tooth advances at 10,000 × 4 × 0.05 = 2,000 mm/min. Feed per tooth is the bite each edge takes; it has a healthy working range for every tool-and-material pair, published by the tool maker just like cutting speed.

Depth of cut: the parameter that travels with them

Feeds and speeds are only half the story: no feed or speed means anything until you say how much material the tool engages. Depth of cut (how far the tool is buried axially) and width of engagement (how much of the diameter is in the cut) set the chip cross-section and the load on the tool. The three together give the material removal rate:

material removal rate = depth of cut × width of cut × feed

which decides how long a job runs. Deeper and wider cuts multiply the load, so tool makers derate the recommended feed per tooth as engagement grows — and eventually the machine’s power and rigidity, not the tool, become the binding limit.

Why speed and feed must be set together

Cutting speed and feed act on different things, which is why they are chosen as a pair. Speed governs temperature at the edge; feed governs how much load each edge carries and how thick the chip is.

As the entry on chip formation explains, a chip that forms and flows properly carries most of the heat of the cut away. Feed too low for the speed makes the edge rub rather than cut: the chip is too thin to form cleanly, heat pours into the tool, and soft material can weld to the edge as built-up edge. Feed too high overloads the edges — deflection, chatter and breakage. Speed too high accelerates flank wear and cratering; speed too low invites built-up edge and a torn finish. The signature of a well-set pair is the chip: crisp, consistent chips in a steady stream, not dust from a timid cut or squealing loads from an aggressive one.

Where the starting numbers come from — and how CNC uses them

Nobody should guess feeds and speeds. Tool makers publish a starting surface speed and feed per tooth for each tool-and-material pair, and handbooks and feeds-and-speeds calculators — including those built into most CAM systems — package the same data. The sequence: look up surface speed and feed per tooth, work out the rpm, multiply up to the feed rate, then set a depth and width of cut the machine can drive, reducing the feed per tooth for deeper or wider cuts.

On a CNC machine that arithmetic ends up as two codes in the program: the spindle speed (S word) and the feed rate (F word). The controller does not choose them — the programmer does — and the machine then holds them exactly, run after run. During prove-out the machinist nudges both live with the spindle and feed overrides, watching chips and listening for chatter, before baking the final numbers into the program.

Mistakes that cost time and tools

• Treating a table as gospel. A feed-and-speed table gives a region to start in, not a value to defend — machine rigidity, spindle and workholding decide the final number.
• Turning the wrong knob. Changing tool diameter means changing rpm to hold cutting speed; feed per tooth is a separate decision.
• Going timid “to be safe”. An over-low feed per tooth rubs, heats and dulls the tool faster than a moderate, chip-forming cut.
• Ignoring chip thinning. When the tool engages well under half its diameter, each edge takes a thinner chip than programmed; feed must rise to restore the bite, or the edge rubs.
• Forgetting the machine’s limits. If good cutting speed needs more rpm than the spindle has, the honest answer is a lower cutting speed and a slower job.

Feeds and speeds are where the physics of the cut becomes numbers in a part program — the bridge between CNC machining, which runs the cut, and chip formation, the physics underneath it.