What Is Feed in CNC Machine Work?

• 1
  Feed Is Distance per Tooth, Not Just a Speed Number
• 2
  What Feed Does Inside the Cut
• 3
  How Feed Is Chosen for a Real Part
• 4
  When Feed Should Stay Low, and When It Should Not
• 5
  Reading Feed Problems from the Part
• 6
  Feed Units Compared

Consider a lathe. Feed is written there as distance per revolution, for example 0.2 mm/rev, because the tool advances once per spindle turn. A mill usually shows distance per minute instead, such as 1,200 mm/min, since a multi-tooth cutter is always in contact. Both numbers describe the same physical idea: how far the cutting edge travels along the workpiece in a given slice of time. That distance is what forms the chip.

The number on the control panel is not the whole story. What actually reaches the cutting edge is feed per tooth, often called chip load. Divide the table feed by spindle speed and by the number of flutes, and you get the thickness of material each edge bites off. A 12 mm three-flute end mill running at 8,000 rpm and 1,200 mm/min removes 0.05 mm per tooth. Too thin and the edge rubs instead of cuts. Too thick and it breaks.

This is why machinists care about feed in a CNC machine more than almost any other setting. Spindle speed controls the cutting temperature. Feed controls the mechanical load on the edge, the tool holder and the part. Change the feed and you change the chip, the forces and the heat balance all at once.

Units matter here. Feed per tooth is written in mm/tooth or inches per tooth. Feed per revolution appears as mm/rev or IPR. Feed per minute shows up as mm/min or IPM. Mixing them up is one of the most common programming errors we see in incoming NC files, and it usually ends in a broken tool or a scrapped part.

Every cutting edge has a minimum chip thickness below which it cannot shear material cleanly. Push the feed too low and the edge ploughs, burnishes and rubs. Heat builds in the tool instead of leaving with the chip. The result looks fine for the first fifty parts, then the tool fails early and the surface turns shiny and torn.

Push the feed too high and the opposite happens. Cutting forces rise, the tool deflects, and a long end mill starts to chatter. On thin walls the part itself moves away from the cutter. Dimensions drift, corners round over, and the finish shows regular marks spaced at the tooth frequency.

There is a useful window in between. Inside it, the chip carries most of the heat away, cutting forces stay steady, and tool wear is gradual and predictable. Finding that window is what feeds and speeds tables are for. They are starting points, not answers.

Feed also interacts with radial and axial depth of cut. A light radial pass with full axial depth keeps the chip thin on the wall but spreads load along the flute, which suits high-efficiency milling. A heavy radial pass with shallow depth concentrates load at the tip and suits roughing where rigidity allows. Feed, radial engagement and axial depth move together.

Start from the material. Aluminum 6061 and 7075 tolerate high chip loads and fast table feeds. Stainless 316 and 17-4PH work-harden if the edge rubs, so the feed must stay above the rubbing threshold even when the surface finish target is fine. Titanium Ti-6Al-4V conducts heat poorly, so the feed has to keep the chip thick enough to carry heat away. Plastics cut clean at high spindle speed but need feed rates that stop melting and stringing.

Then look at the tool. Carbide grades with a coating such as AlTiN run faster than uncoated HSS. Flute count sets the chip load per tooth: a four-flute cutter at the same table feed takes a smaller bite per edge than a two-flute tool. Long tools with a high length-to-diameter ratio need the feed reduced, or the deflection will show up in the wall.

Then the setup. A part held in a vise on a 3-axis machine behaves differently from one on a Ø400 mm rotary table in a 5-axis cell. Overhangs, workholding stiffness and the number of setups all push the safe feed down. On our 16 simultaneous 5-axis centers, we often trade a small feed reduction for fewer setups, which usually wins on total cost.

Finally, the finish requirement. Roughing runs at the highest feed the setup allows, with finish left for a separate pass. Semi-finishing uses a moderate feed to leave a consistent stock allowance. Finishing runs at a feed low enough to hit the surface target, but not so low that the edge rubs. On aluminum, a finishing feed around 0.05 to 0.10 mm/tooth with a sharp uncoated cutter reaches Ra 0.8–1.6 μm without extra polishing.

Thin walls and fine features are the clearest case for lower feed. A 0.8 mm wall in aluminum will deflect under a heavy finishing pass, so the feed drops and the number of passes rises. Small tools follow the same rule. A 1 mm end mill snaps long before the machine reaches its feed limit.

Deep pockets and long-reach tools also argue for restraint. As the tool sticks out, its stiffness falls sharply. Chatter appears first as a faint pattern on the floor of the pocket, then as noise and a poor finish. Reducing feed and adjusting spindle speed together usually clears it. Dropping feed alone often makes it worse, because the chip gets thinner and the edge rubs.

Heat-resistant alloys are the case where low feed is the wrong answer. Inconel and similar nickel alloys work-harden the surface if the edge dwells. The fix is a heavier chip load, not a lighter one, plus enough rigidity to carry it. That is counterintuitive for engineers used to aluminum, and it is the reason we ask for the material grade before quoting a cycle time.

Hardened steel above 45 HRC sits in a separate category. Feeds stay moderate, depths stay shallow, and the cutter is usually a coated carbide or CBN tool run on a machine with good thermal stability. Pushing feed here buys cycle time at the cost of tool life, and the trade is rarely worth it on small batches.

Regular marks spaced evenly around a bore or along a wall point to chatter, not to a feed that is simply too fast. Count the marks per revolution and compare them with the flute count. If they match, the tooth frequency is showing up in the surface, and the fix is usually a change in spindle speed combined with a feed adjustment.

A shiny, burnished surface with a good-looking profile is the classic sign of a feed that is too light. The edge is rubbing rather than cutting, and tool life will fall even though the part looks acceptable. Increasing feed per tooth and checking the chip shape usually confirms it. Healthy chips are thick and break cleanly; dust and fine powder mean the feed is too low.

Color in the chip tells you about heat. Straw-colored steel chips are normal. Blue or dark gray chips mean the cutting zone is too hot, which usually calls for a lower feed or a different coating rather than a higher spindle speed. Aluminum chips that weld to the edge signal a build-up problem, often solved with a polished flute and a slightly higher feed.

Burrs on the exit edge of a cut have their own logic. A moderate feed leaves a small, consistent burr that deburring tools remove quickly. Too light a feed smears material and creates a thin, hard burr that is difficult to remove. Too heavy a feed pushes a large burr that can chip the edge on the next pass.