The feed that reaches the machine

Every bit in the tool database carries a feed rate and a plunge rate. Those two numbers are what the toolpath is built from: the strategy asks the bit for them, stamps them on every cutting move it generates, and the post writes an F word once and then only when the rate changes. A plain profile around a rectangle comes out as two F words for the whole operation — one for the plunge, one for the cut — and both are the bit’s own.

That is the floor. Everything below is what can happen on top of it, and all of it is optional.

The material usually has the better number

A feed written against a bit is what that bit likes in general, and “in general” is not a material. The material database holds a feed, plunge, spindle speed, stepover and stepdown for each tool shape in each stock you cut, so picking a 6 mm end mill for a job in oak fills the operation with the oak numbers rather than the bit’s all-purpose ones. The form says which of the two it is showing you.

Where the material has nothing to say for that shape of bit, the figures are computed instead — from the diameter and flute count, the stock, the strategy being run, and the active machine’s spindle range and maximum feed. Anything the machine cannot deliver is clamped to what it can, and the status bar names the material, the feed, the speed, the plunge and the depth of cut every time a toolpath is calculated, along with whichever figures had to be clamped. You are not asked to trust it; you are told what it used.

Why the feed then moves along the path

One feed for a whole operation is a compromise: it has to be slow enough for the worst moment on the path, which means it is too slow for the rest of it. With auto feeds on, each move is set against its own conditions rather than against the worst case.

• On a light radial cut the chip is thinner than the feed per tooth suggests, so the feed goes up rather than down — the cutter is rubbing, not cutting, if it does not.
• Into an internal corner the engagement climbs sharply as the tool meets material on two sides at once, so the feed eases off before the corner rather than after it.
• Around an arc the tool centre and the cutting edge do not travel the same distance, so the programmed feed is compensated for the difference — it is the cutting edge that should be moving at the rate you asked for, not the machine’s centreline.

The important part is what it is calculated against. Each move’s own nominal feed — the one from your tool or your material — is the reference, and the result is bounded both ways: it cannot fall below a fraction of it, cannot rise above a multiple of it, and is then clamped again to the machine’s own limits. It is a modulation around your number, not a substitute for it.

A 6 mm end mill set to 1800 mm/min with a 600 mm/min plunge, profiling a rectangle, posts as F600 down, F1800 along the first run, and F900 through the square corners. The plunge is not touched. Turn the option off and the same path posts as F600 and F1800, and nothing else.

Using your own numbers instead

Auto feeds and speeds is a single tick in the Machine menu. With it off, nothing is recomputed and nothing is modulated: the feed, plunge and speed on the operation are written into the file exactly as they stand. There is no separate mode to learn and no second set of fields — the numbers are the same numbers, they are simply left alone.

Which means the way to set your own feed is to write it where the feed lives. Put it on the bit in the tool database if it is how you always run that cutter, or on the material row if it is how you run that cutter in that stock. Both are a field and a Save, and both are what the next job will start from as well as this one.

The numbers that were always yours

Auto feeds touches three figures and no others: feed, plunge and spindle speed. Everything that decides how the tool gets into the material and how much of it comes off per pass is an operator control and is never written over.

• Entry: a straight plunge or a ramp, and the length the ramp runs over.
• Stepdown — the depth taken per pass — and stepover, the advance between passes.
• The last pass: its allowance, and whether it runs in the opposite direction.
• Tabs, lead-ins and lead-outs, and the order the operations run in.

So a ramp entry over 20 mm stays a ramp entry over 20 mm whether the option is on or off. What changes is only the rate the tool travels while it does it.

In Carvect: the tick is Machine ▸ Auto Feeds & Speeds. The numbers themselves live in Setup ▸ Tool Database, per bit, and Setup ▸ Material Database, per material and tool shape — the material’s row wins where it has one. Entry mode and ramp length sit on the toolpath form beside the depth settings, and the status bar reports the feeds used, and any that were clamped, each time a toolpath is calculated.