GCarve

GCarve

CNC router feeds and speeds, from the bit you bought

You don't need to work out feeds and speeds yourself. In GCarve you pick the bit you bought by maker and part number; the maker's chip load comes with it from our database of 29,500+ bits, and GCarve turns it into spindle speed, feed, plunge and depth per pass for your material, kept inside what your machine can do. A meter then shows whether the numbers you type are in the sweet spot.

How it works

  1. Pick your machine in Board settings, from 2,100+ CNC routers: its spindle speed range, top feed and plunge rates come with it.
  2. Pick your material: softwood, hardwood, plywood, MDF, plastics, aluminium or foam (the material name is enough: "Baltic birch" counts as plywood).
  3. Pick your bit: Tool Library ▸ Browse bit catalog, by maker and part number. 16,312 bits carry their maker's chip loads (Amana, Onsrud, Whiteside, Vortex and others); browse them in the router bit database.
  4. Read the numbers: GCarve fills in RPM, feed, plunge and depth per pass. Change any of them and the chip-load meter moves from "rubs and burns" to "breaks the bit".

The formula

Feed = RPM × flutes × chip load. The chip load is how thick a chip each cutting edge takes (inches per tooth). Too thin and the bit rubs, heats up and burns the wood; too thick and it chatters, leaves a rough edge or breaks.

Example: a ¼ in 2-flute end mill in plywood, with no maker chip load, gets GCarve's chart value of 0.011–0.013 in/tooth. At 18,000 RPM the middle of that range is 18,000 × 2 × 0.012 = 432 in/min on an industrial router. On a hobby machine GCarve takes 35 % of that chip load (151 in/min) and half the pass depth, and then caps the feed at the machine's top speed.

Your machine changes the numbers

Maker charts assume a heavy industrial router. Lighter machines flex, so GCarve scales the chip load and the depth per pass by the machine's class:

Machine classChip load usedDepth per pass used
Industrial (or none picked)100 %100 %
Prosumer60 %75 %
Hobby35 %50 %
Desktop and handheld30 %40 %

Then the limits: spindle speed stays inside the machine's range and under the bit's own maximum; when the spindle can't turn slower, the feed goes up to keep the chip load; feed and plunge never pass the machine's top rates. A pass deeper than the bit is wide lowers the target: 80 % at twice the diameter, 60 % from three times.

GCarve's chip-load chart (when the maker has none)

Inches per tooth, low–high, at three bit diameters; sizes in between are interpolated. A V-bit is treated as a ⅛ in bit at most, since it cuts with its narrow tip.

Material⅛ in bit¼ in bit½ in bit
Softwood0.004–0.0060.009–0.0110.019–0.021
Hardwood0.003–0.0050.008–0.0100.016–0.018
Plywood0.004–0.0060.011–0.0130.021–0.023
MDF0.004–0.0070.011–0.0130.021–0.023
Plastics0.002–0.0040.004–0.0060.010–0.012
Aluminium0.001–0.0020.003–0.0040.006–0.008
Foam0.006–0.0080.012–0.0150.025–0.030

Before you cut

Every number is a starting point. Listen to the cut, look at the chips (fine dust means too slow, a squeal means too fast or too deep), and check the maker's current data for a new bit. GCarve's export also warns when a cut is deeper than the bit's flutes or the job goes past your machine's limits, and an air-cut file lets you run the job above the board first.

Related: how to V-carve, router bit database, CNC machine database, GCarve vs VCarve.

Questions

What are feeds and speeds on a CNC router?

The spindle speed (RPM), how fast the bit moves sideways (feed, in/min or mm/min), how fast it plunges, and how deep each pass goes. Together they set the chip load: how thick a chip each cutting edge takes.

How do I calculate the feed rate?

Feed = RPM × number of flutes × chip load. A 2-flute bit at 18,000 RPM with a 0.005 in chip load feeds at 18,000 × 2 × 0.005 = 180 in/min.

Do I need a feeds and speeds calculator?

Not with GCarve. Pick the bit you bought by maker and part number and the speed, feed, plunge and depth per pass are worked out for your material and machine from the maker's own chip load.

What chip load should I use?

The bit maker's, for your material and bit size: it is printed in their catalog or feed chart, and GCarve already has it for 16,312 bits. Without one, GCarve uses its own chart by material and diameter (see the table above).

Are maker feeds safe on a hobby CNC?

Maker charts assume a rigid industrial router. GCarve scales them down for lighter machines (hobby machines start at 35 % of the chip load and half the pass depth) and never goes past your machine's top feed or spindle speed.

What if my bit isn't in the database?

Add it in the Tool Library with its type, diameter and flutes, or import your Vectric .vtdb or Fusion 360 tool library. GCarve then uses its own chip-load chart for that size and material.

Try it on your own job: GCarve is free, runs in your browser with a free account, and has free desktop apps.

Open GCarve free