The Relationship Between Cutting Speed, Feed, Depth of Cut and Spindle Power

• 1
  What the relationship between cutting speed and the other three variables actually means
• 2
  The formulas and what each one is for
• 3
  The order to set the variables, and why the order matters
• 4
  How the relationship between cutting speed and finish changes across passes
• 5
  Where the formulas stop being useful
• 6
  Starting cutting data by material and operation

Four numbers describe a turning or milling pass: cutting speed (vc), feed (fz per tooth or f per revolution), depth of cut (ap) and stepover or width of cut (ae). Spindle speed n is derived from vc, not chosen separately. The relationship between cutting speed and feed is the one that decides most of your tool life, because both raise the temperature at the cutting edge.

Cutting speed is surface speed, not rpm. A Ø50 mm face mill at 300 m/min runs at roughly 1,910 rpm. The same 300 m/min on a Ø6 mm end mill needs about 15,915 rpm, which most 40-taper spindles cannot reach. That single fact is why small tools are usually run below the recommended vc and large tools at or above it.

Feed per tooth sets the chip thickness. If the chip gets too thin, the edge rubs instead of cutting, work-hardens the surface and wears faster than it would at a heavier feed. This is the counterintuitive part: raising feed per tooth within the insert's range often extends tool life, while raising cutting speed almost always shortens it.

Depth of cut decides how many passes the job takes; stepover decides how much of the cutter is engaged. Together they set the chip load the tool body and the fixture have to absorb. None of these four can be set in isolation, and none of them can be read off a chart without checking what the machine and the setup can carry.

Spindle speed follows directly from cutting speed: n = 1000 × vc / (π × D), with vc in m/min and D in mm. For imperial work, n = 3.82 × vc / D with vc in sfm and D in inches. Everything downstream depends on n being right, so this is the first number to calculate.

Table feed comes from the tooth count: vf = fz × z × n, where fz is feed per tooth in mm and z is the number of effective teeth. On a 4-flute cutter at 8,000 rpm with fz = 0.05 mm, table feed is 1,600 mm/min. If the controller or the tool holder cannot hold that feed accurately, reduce fz rather than the rpm.

Machining time for a straight pass is tc = L / vf, with L the total travel including approach and overrun. Add 10–15% for acceleration and deceleration on short moves. For a pocket, estimate path length first; the formula has little value if you guess the path.

Spindle power is the check that most programmers skip. A working estimate is Pc = ap × ae × vf × kc / (60 × 10^6) kW, with kc the specific cutting force in N/mm². For 6061-T6 aluminium, kc is around 700–900 N/mm²; for 1045 steel it is roughly 1,700–2,100 N/mm²; for 316L stainless it climbs to 2,200–2,600 N/mm². Compare Pc with the spindle's continuous rating, not its peak rating, and keep the result below about 80% of continuous power.

• 1
  n = 1000 × vc / (π × D)Spindle speed from surface speed and diameter.
• 2
  vf = fz × z × nTable feed from feed per tooth, tooth count and rpm.
• 3
  tc = L / vfCutting time for a known path length.
• 4
  Pc = ap × ae × vf × kc / (60 × 10^6)Rough spindle power estimate in kW.

Start from the tool. Insert grade and coating define a vc window, and the tool's flute count and core diameter define a practical fz range. A coated carbide insert in P25 grade cutting 1045 steel typically sits between 150 and 250 m/min. Solid carbide end mills in the same material run 100 to 180 m/min. Those windows are the boundary you work inside.

Then set depth of cut from rigidity. The rule most shops use is to take as much ap as the setup allows, then reduce if chatter or deflection appears. On a rigid 50-taper machine with a short tool, that can be 3–5 mm per pass in steel. On a long, slender tool, 0.5 mm is already ambitious. Depth of cut is limited by the weakest link: the tool, the holder, the workpiece or the fixture.

Then set feed per tooth to match the chip load the insert needs. Insert makers publish a starting fz, but the correct value depends on the radial engagement. At light stepover (below 25% of diameter), you can raise fz, because the chip thins as the cutter exits the material. At full-width cuts, keep fz at the published value or slightly below.

Cutting speed comes last, and it is the variable you trim to hit tool life. If the edge fails by chipping, reduce feed or check runout. If it fails by cratering or flank wear, reduce vc. This order is the reverse of how the numbers appear on a chart, and it is the reason two shops using the same insert get different tool life.

Roughing is about removing volume at the lowest cost per cubic centimetre. Here you use high ap and moderate vc, and you accept a surface around Ra 3.2–12.5 μm. The limit is spindle power and tool deflection, not finish. If the blank has 6 mm of stock and the machine can take it, one pass beats three.

Semi-finishing leaves a controlled margin so the finishing pass has a uniform load. A common split is to leave 0.5–1.0 mm radial and 0.2–0.3 mm axial. Running the semi-finish at the same vc as roughing is fine; the point of the pass is to even out the stock, not to improve the surface.

Finishing raises cutting speed and drops feed per tooth to hit the finish callout. To hold Ra 0.8–1.6 μm in aluminium, a typical setup is 400–600 m/min with fz around 0.03–0.05 mm and ap under 0.5 mm. Pushing vc higher risks chatter marks from the higher spindle speed; pushing fz higher leaves visible scallops.

When the print calls for Ra 0.2–0.8 μm, plan on a separate finishing strategy: a smaller stepover (5–10% of diameter), a sharp uncoated or polished tool, and enough coolant or air blast to clear chips. At that level, the relationship between cutting speed and surface finish becomes secondary to tool runout and machine vibration. A 0.01 mm runout will wreck the finish no matter what vc you pick.

The formulas assume a rigid setup with a sharp tool and stable chip evacuation. In a deep pocket with a 4:1 overhang, the tool deflects before the calculated power limit is reached. The deflection limit, not power, sets the depth of cut. A rough check is to keep radial engagement under 10% of diameter when overhang exceeds 4× diameter, and raise feed per tooth to compensate for the thinner chip.

Heat-resistant alloys break the power estimate more often than carbon steel does. Inconel 718 work-hardens within a few micrometres of the surface, so a too-light finishing pass leaves a harder skin for the next operation. In these materials, keep fz above 0.02 mm and never let the tool rub. Cutting speed stays low, often 25–45 m/min, and coolant pressure matters more than flow.

Thin-wall parts add another constraint. A 1.5 mm wall in aluminium will deflect under a 2 mm depth of cut even if the spindle has power to spare. Reduce ap, increase vc slightly, and use climb milling with a high-lead cutter to push the force into the rigid direction.

Finally, the machine's acceleration and the controller's look-ahead set a practical ceiling on feed for 3D contouring. A machine rated at 12,000 mm/min may only hold 3,000 mm/min through tight radii. Watch the feed override on the first part and adjust the program rather than the machine. We run 127 high-precision CNC machines across 5-axis, 4-axis, 3-axis and mill-turn platforms, and the practical feed ceiling differs by platform, not by material alone.