CamCraft

CAM fundamentals

Feeds and speeds

Feeds and speeds are the two numbers that decide whether a cut is fast, clean and survivable: how fast the tool spins, and how fast it moves.

The principles

Surface speed is how fast the cutting edge travels through the material at the tool's outer diameter. It depends on the work material and the tool material, not on the tool size. Chip load (feed per tooth, fz) is how much material each flute takes per revolution. Too little rubs instead of cutting and wears the edge; too much overloads it.

The two formulas that turn them into machine settings:

  • spindle speed: n = Vc x 1000 / (pi x D), with Vc in m/min, D in mm and n in rpm (in inch units, n = Vc x 12 / (pi x D) with Vc in feet per minute and D in inches);
  • feed rate: vf = fz x z x n, with z the number of flutes.

Engagement. Radial engagement (ae, the stepover) is how much of the diameter is in the cut sideways; axial engagement (ap, the stepdown) is how deep. Heavy axial depth with light radial engagement is the usual way to use the full flute length.

Chip thinning. When the radial engagement is less than half the diameter, each flute leaves the cut before it has taken a full-thickness chip. The real chip is thinner than fz. For a square-shouldered cut the ratio is 2 x sqrt(r - r^2), with r = ae / D. To keep the intended chip thickness at light stepovers, raise the programmed feed by the inverse of that ratio. The compensation has a limit: at very light stepovers the factor runs away, so it is held.

Plunge and ramp feeds. Plunging loads the tool axially, where an end mill is weakest and chips cannot escape, so plunge feed is much lower than cutting feed. A ramp or helix entry spreads the descent over a longer path.

Reading the cut. A steady, even sound is right. A scream or chatter means speed or engagement is wrong. Chips should come off as clean, uniformly coloured curls. Blue or dark chips in steel, or melted, welded chips in aluminium, mean too much heat for the feed. These are cues for the first cuts, not numbers.

A less rigid machine needs less engagement and a lower feed before it needs a lower speed. Lighter radial engagement is usually the first change.

What CamCraft does

On an operation's Feeds tab:

  • Spindle speed is shown and editable as rpm, or as surface speed through the tool's diameter: m/min in a millimetre document, surface feet per minute (SFM) in an inch one. The speed lives on the tool.
  • Feed and Plunge feed are separate numbers on the operation.
  • Climb milling is a check box (see Toolpath strategy).
  • The Cutting data group holds the document's workpiece material, the tool's edge material (HSS or carbide) and flute count. With all three stated, Suggest feeds & speeds shows a starting rpm and feed from the formulas above. Nothing changes until you click Apply suggestion, and the apply is one undoable step.
  • The suggestion's numbers come from a small built-in table of workpiece groups (steel, stainless, cast iron, non-ferrous, plastics) with conservative starting values. They are a starting point, not a limit. The table does not speak for every tool kind: it says so by name when it cannot suggest.
  • Chip thinning compensation is applied only where the operation states an optimal engagement load. Adaptive clearing does.
  • Lathe tools can state a constant surface speed and a feed per revolution; the post then writes constant surface speed with a maximum-rpm clamp.

Limits CamCraft enforces. The suggestion is clamped to the mounted machine's stated spindle range and feed ceiling, and each clamp is named in the suggestion. Independently, the program gate refuses to post an operation whose tool runs above or below the machine's stated rpm, and one whose estimated spindle power exceeds the machine's stated power (only when the machine, material, flutes and engagement are all stated; CamCraft makes no claim from an unstated number).

A lathe setup can also state a workholding rpm limit (the chuck or collet rating). Under constant surface speed the rpm ceiling becomes the lowest of the machine's, the tool's and the workholding's. Under constant rpm, an operation over that limit is refused by name, not capped, because the cut was planned at that speed. The limit is lathe-only; mill setups have no equivalent setting. See Setups and Workholding.

CamCraft does not measure sound or chip colour and does not model machine rigidity. The first cut is where you learn whether the numbers fit.