Cutting Speed Guide

What cutting speed actually measures

Cutting speed (V_c) is the surface speed at the cutting edge — how fast the periphery of the tool moves through the material, expressed in metres per minute. It is not the spindle speed. A ⌀6 mm tool and a ⌀16 mm tool turning at the same RPM are cutting at completely different speeds, which is why a shop that thinks in RPM alone will burn small tools and under-drive large ones.

Cutting speed matters because it governs the temperature and the wear mechanism at the edge. Below the useful range the edge rubs rather than shears, work-hardening the surface and producing a built-up edge. Above it, the edge softens, the coating degrades and flank wear accelerates sharply. The useful window is a property of the material-and-tool pair, not of the machine.

Imperial shops express the same quantity as surface feet per minute (SFM). The conversion is direct: 1 m/min = 3.281 SFM, so a Vc of 120 m/min is about 394 SFM.

The two formulas

One relationship, written two ways. Use the first when you know the spindle speed and want the cutting speed; use the second — far more often — when you have chosen a cutting speed and need the RPM to programme.

The factor of 1000 converts millimetres to metres; π×D is simply the circumference the edge travels once per revolution.

Worked example

A ⌀10.0 mm end mill, with a target cutting speed of 120 m/min taken from the tool manufacturer's data for the workpiece material in question:

Reverse the calculation to sanity-check a programme you have inherited. The same tool running at 8 000 RPM is cutting at 251 m/min — which may be entirely correct in aluminium and entirely wrong in a hardened die steel. The number to compare against is always the material's, never the machine's maximum.

Effective diameter — the mistake that costs corner radii

The D in the formula is the diameter actually engaged in the cut, not the diameter stamped on the shank. Three common cases where they differ:

• Shallow cuts with a ball nose. At an axial depth well under the tool radius, only a small band near the tip is cutting, and the effective diameter can be a fraction of the nominal. Programming nominal diameter here means the tip is rubbing, not cutting.
• Corner-radius tools taking a light axial pass. If ap is smaller than the corner radius, the engaged diameter is reduced by the radius geometry. The reduction is modest but real, and it lands exactly on the part of the edge that is hardest to replace.
• Tilted or five-axis contact. Any lead or tilt angle moves the contact point and changes the engaged diameter continuously along the toolpath.

Substitute D_eff for D in the RPM formula. On a ⌀10 mm ball nose taking a 0.5 mm axial pass, D_eff is 4.36 mm — the spindle speed for a given cutting speed is more than double the nominal figure. This single correction is the most common reason a finishing pass leaves a poor surface.

General industry starting ranges by ISO group

The ranges below are the broad, publicly established bands used across the milling industry for solid carbide tooling. They exist to tell you the order of magnitude — whether the answer is 60, 200 or 800 m/min — not to set your programme.

Ranges vary widely by alloy, condition, coating, engagement and coolant strategy — a single ISO group spans materials that behave very differently. Always prefer the tool manufacturer's data for the specific tool over any general band.

Two structural points hide inside that table. First, the N group is limited by how fast chips can leave the flute, not by heat — which is why the ceiling is set by the spindle and the chip evacuation strategy. Second, the S group's low speeds are not timidity: the heat generated in nickel alloys stays in a very small zone at the edge, and speed is the parameter that concentrates it.

When to reduce the calculated speed

The calculated figure assumes a rigid, well-supported cut. Reduce it when the assumption fails:

• Long reach. Deflection rises with the cube of unsupported length; a tool at 5×D stickout is a different tool from the same one at 2×D.
• Thin-wall or unsupported workpieces, where the part rather than the tool sets the limit.
• Interrupted cuts — cast surfaces, cross-holes, weld beads — where the edge takes repeated mechanical shock rather than steady load.
• Full-slot cutting, where heat cannot escape and the chip has nowhere to go. See the Step-Over Guide.
• Marginal holding — a long collet extension, a worn holder or measurable runout. Runout multiplies the load on whichever edge is running high.

Conversely, the case for increasing speed is usually a case for changing strategy instead: a lighter radial engagement at a higher speed and a proportionally corrected feed removes more material per minute than a heavy slot at a cautious speed, and does it with less heat in the edge.