Feeds, Speeds & Toolpaths

Two settings sit at the heart of every cut. Spindle speed is how fast the bit rotates, measured in RPM (revolutions per minute) - typically 10,000-24,000 on a router, much lower on a metal-cutting mill. Feed rate is how fast the machine drives the bit through the material along the toolpath, measured in mm per minute (or inches per minute). Spindle speed is the spin; feed rate is the travel. They are set independently, but they only make sense together.

Why together? Because what actually matters to the cutting edge is not either number alone but their relationship - how much material each edge removes per revolution. Spin fast and travel slow, and each edge shaves a whisker: the bit rubs, generates heat by friction, and burns. Spin slow and travel fast, and each edge tries to gouge a huge bite: forces spike, the bit deflects and can shatter. The correct cut lives in between, where each edge peels a chip of a sensible thickness. That thickness has a name, and it is the key that unlocks the whole subject.

Chip load (or feed per tooth) is the thickness of material each cutting edge - each flute - removes in one pass. It is the quantity feeds-and-speeds actually aim to control, and the relationship is simple and worth memorising:

feed rate = RPM x number of flutes x chip load.

Read it as a recipe. If a 2-flute bit spins at 18,000 RPM and its recommended chip load in this material is 0.1 mm per tooth, then feed rate = 18,000 x 2 x 0.1 = 3,600 mm/min. Change the bit to 3 flutes and the feed rises to 5,400 mm/min for the same chip load, because more edges share the work. This is why flute count matters: more flutes let you feed faster (or cut smoother) at the same chip load, but leave less room to clear chips. Manufacturers publish recommended chip loads per bit diameter and material - that is your starting point, not a table to obey blindly.

The deeper idea is why a proper chip matters. A real chip carries heat away with it as it flies off; a too-thin shaving does not, so the heat stays in the bit and the workpiece and you get burning and premature tool wear. A too-thick chip overloads the edge. So the goal of tuning feeds and speeds is always the same: make a real chip - not dust, not a jam. If your cut is producing fine powder and smoke, feed faster or slow the spindle; if it is straining, chattering or throwing the bit, back off. You are steering the chip.

You almost never cut a shape in one go. Real work splits into at least two strategies. A roughing pass removes the bulk of the waste as fast as possible with a big bit, coarse settings, and deep bites, and it deliberately leaves the surface rough and slightly oversized - a thin stock allowance (say 0.3-0.5 mm) standing proud of the final line. Roughing does not care about finish; it cares about clearing material quickly and safely, so it takes the deepest, most aggressive cuts the machine and bit can stand.

A finishing pass then comes back with a smaller, sharper bit (a ball nose for curved surfaces) and fine settings to skim that leftover allowance down to the exact final surface, leaving it smooth. Because it removes only a whisker, it can afford small, precise steps and a slow, clean feed. Two toolpath parameters govern all of this. Stepdown (or depth of cut) is how deep each pass goes in Z - big for roughing, so you clear material in a few thick layers; there is a rule of thumb that a single stepdown should not exceed roughly the bit diameter, and far less in hard material. Stepover is how far the tool shifts sideways between adjacent passes - wide for roughing (fast, leaves ridges), tiny for finishing (slow, leaves a mirror-smooth surface with barely visible scallops). Roughing is about volume; finishing is about the last fraction of a millimetre.

Feeds and speeds set how fast; the toolpath sets how the tool moves, and it matters as much for tool life as the numbers. First, how the tool gets into the material. Dropping a bit straight down at full depth - a plunge - is hard on it, because the centre of an end mill barely cuts and mostly rubs. Better entries ramp the tool in at a shallow angle or spiral it down in a helix, so it shears material as it descends rather than pounding straight in; CAM offers these, and using them dramatically reduces breakage on pockets.

Second, the direction of cut. In climb milling the cutting edge enters at full chip thickness and thins to nothing, giving a cleaner finish and less rubbing - the default for finishing on a rigid CNC. In conventional milling the edge starts at zero and thickens, rubbing at the start of each chip; it is gentler on flimsy setups but leaves a rougher surface. Third, modern CAM offers adaptive or high-efficiency clearing for roughing: instead of full-width cuts that bury the bit in a corner, the toolpath keeps the tool engagement constant and shallow but takes a deep stepdown, letting you rough faster with less heat and longer tool life. Finally, small touches make a big difference: keep the tool cutting rather than dwelling in one spot (dwelling burns), lead in and out of a finished edge smoothly rather than diving straight at it, and set safe retract heights so rapid moves never clip the work. The chip-load numbers get you a safe cut; the toolpath strategy is what makes it clean, fast and gentle on the bit.

Reason one through. Say you are cutting a pocket in plywood with a 6 mm two-flute flat end mill on a router. The bit maker suggests a chip load around 0.1 mm per tooth for wood at this diameter, and the bit is rated to a high RPM. Pick a spindle speed - 18,000 RPM is a sensible middle. Now the feed follows directly: feed = 18,000 x 2 x 0.1 = 3,600 mm/min. For the stepdown, a conservative first attempt might be half the bit diameter, so 3 mm per pass, cutting a 12 mm-deep pocket in four passes. For roughing you might set stepover to ~40 percent of the diameter (about 2.4 mm) to clear fast; for a finishing wall pass, a light stepover for a clean edge. Those are starting numbers - you then listen: a clean cut sounds crisp and throws chips; a scream or smoke says slow the feed or the spindle; a strained groan says the bite is too deep, so reduce the stepdown.

Why does this matter so much? Because the failure modes are expensive. Feed too slow / RPM too high: the bit dwells and rubs, heat has nowhere to go, and wood burns (those brown scorched edges), plastic melts and re-welds behind the bit, and the tool dulls fast. Feed too fast / stepdown too deep: cutting forces exceed what the bit can take, it deflects and then breaks - often flinging pieces and ruining the part. Both extremes also worsen surface finish and can pull the workpiece loose. Getting feeds and speeds right is not fussiness; it is the difference between a finished part and a scrapped one, a sharp bit and a snapped one. Start from the manufacturer numbers, cut a test in scrap, read the chips and the sound, and adjust.