Feed Rate Guide

Feed per tooth is the real parameter

The number that matters at the cutting edge is the feed per tooth (f_z), also called the chip load: the thickness of material each individual edge removes per revolution. Table feed (v_f) is what the machine is told, but it is a consequence of three things — chip load, tooth count and spindle speed — and only one of them is a property of the cut.

There is a floor as well as a ceiling. Below a minimum chip thickness the edge cannot form a chip at all: it deflects the material elastically, ploughs through it and springs back. That produces heat instead of chips, work-hardens the surface, and is the mechanism behind a surprising share of "the tool was no good" failures. On a five-flute tool at a light radial engagement, the actual chip thickness can be a small fraction of the programmed feed per tooth — see chip thinning below.

The formulas

Note what z does. Two tools of the same diameter running the same chip load at the same cutting speed will have very different table feeds if one has three flutes and the other five. That is the entire commercial argument for higher flute counts — more edges carrying the same load per edge — and it holds only while the chips can still escape and the machine can still deliver the feed.

Worked example

Continuing the ⌀10.0 mm example from the Cutting Speed Guide: 3 820 RPM, five effective flutes, and a feed per tooth of 0.05 mm taken from tool data for the material.

Now check it the other way. If the same tool is being run at 400 mm/min "to be safe", the actual chip load is 0.021 mm per tooth — probably below the minimum chip thickness for the geometry, and therefore the least safe option available.

Chip thinning — radial

When the radial engagement (a_e) is less than half the tool diameter, each edge enters and leaves the material along an arc, and the chip it produces is thinner than the programmed feed per tooth. The tool is doing less work than the numbers say, and the correction is to feed faster, not slower.

Rearranged into the form used in practice — the corrected feed needed to keep a target chip thickness:

The factor is pure geometry — it applies to any tool at that engagement ratio. It does not license exceeding the tool's maximum chip load, the machine's feed capability, or the point at which the surface finish degrades.

This is the calculation behind high-efficiency milling: a light radial engagement at a heavily corrected feed keeps the chip thick enough to cut, spreads wear along more of the flute length, and keeps heat in the chip rather than in the edge.

Chip thinning — axial and lead angle

The same effect occurs axially. A round-insert or corner-radius tool taking an axial depth smaller than the corner radius spreads the chip over a longer contact arc, thinning it. A tool with a lead angle does the same by geometry: the chip thickness is the feed multiplied by the cosine of the lead angle, so a 45° lead produces a chip roughly 0.71 times the programmed feed — and correspondingly allows a higher feed for the same chip thickness.

In practice: if you reduce the axial depth for a finishing pass and leave the feed where it was, you have quietly moved the edge towards the rubbing regime. Reduce the depth and raise the feed, or accept the finish penalty knowingly.

Climb and conventional milling

Direction of cut changes the chip the edge sees, which changes the feed that makes sense.

• Climb milling (down milling) starts each chip at maximum thickness and ends at zero. Heat leaves with the chip, the surface finish is generally better, and cutting forces push the workpiece into the fixture. It is the default on any machine with a preloaded ball screw and no backlash.
• Conventional milling (up milling) starts the chip at zero thickness — the edge rubs before it cuts, which raises heat and work-hardens the surface ahead of the next tooth. It remains appropriate on machines with backlash, on hard scaled surfaces such as castings and forgings, and where a climb cut would pull the part out of a weak fixture.

Corners deserve separate attention: as a tool sweeps an inside corner, the radial engagement rises sharply for a moment even though the programmed a_e has not changed. The chip goes from thin to thick within a fraction of a revolution. Either reduce the feed through the corner in the programme, or — better — use a corner-rounding toolpath so the engagement never spikes.

Reading the chips

Chips are the cheapest diagnostic available. A correctly loaded cut in steel produces chips that leave the flute cleanly, curl consistently and are warm rather than glowing.