CNC feeds and speeds explained: the whole picture
Short answer
Feed rate is how fast the tool moves. RPM is how fast it spins. Together with the flute count they set the chipload, which is the actual thickness of each chip. Depth and stepover then decide how much of the tool is buried. Get the chipload right first, then adjust depth and stepover to whatever your machine can hold without flexing.
Five numbers, and what each one controls
| Number | What it is | What it mainly affects |
|---|---|---|
| Spindle speed (RPM) | How fast the tool rotates | How often an edge hits the material |
| Feed rate | How fast the tool travels sideways | How far the tool moves between those hits |
| Flute count | How many cutting edges the bit has | How many hits happen per revolution |
| Depth per pass | How deep each pass cuts, along Z | How much of the tool's length is loaded |
| Stepover | How far sideways between passes | How much of the tool's diameter is buried |
The first three combine into one number, the chipload, which is the thickness of the chip each edge takes. That number is the one that decides whether you are cutting or rubbing. The last two decide how hard the machine has to push, which is what decides whether it flexes, stalls or breaks something.
Why nobody can just give you the number
You will see people ask for "the settings for walnut" and get ten different answers, all of them honest. That is because at least nine things move the right answer:
- Machine rigidity. A heavy steel frame and a light aluminium extrusion frame do not cut the same, ever.
- Router or spindle. A trim router loses torque badly at low RPM. A VFD spindle holds it, which changes which RPM is available to you.
- Minimum RPM. Many trim routers will not go below about 10,000, which sets a floor on feed rate for a given chipload.
- Bit diameter. A 1/8 inch bit cannot take the chip a 1/2 inch bit can, and it deflects far more.
- Flute count. Two flutes need twice the feed of one flute for the same chip thickness.
- Bit quality and sharpness. A dull bit needs more force for the same cut, and generates far more heat.
- Material. Not just species. The same board can machine differently across a knot, near the pith, or when it is wet.
- Workholding. A part that flexes under the cut changes the effective depth continuously.
- Chip evacuation. A cut full of its own chips behaves nothing like a clear one.
What to do instead of asking for the number
Ask for a starting point, run it on scrap, and read the result. Chips, sound, heat and finish all tell you which direction to move. That skill transfers to every material you will ever cut. A borrowed number does not.How to set feeds and speeds, in order
- Start with the bit maker's chart if you have one. They tested the geometry you are holding. Use their chipload range for your material and diameter.
- Pick an RPM your machine likes. For most hobby routers in wood that is somewhere in the middle of the dial rather than flat out. Flat out is loud, hot, and usually means you then need an unreachably high feed rate.
- Calculate the feed rate from the chipload, RPM and flute count.
- Pick a depth per pass your machine can hold. Depth per pass is the setting to back off first when the machine complains.
- Run it on scrap and read the cut. Then change one thing at a time.
Reading the cut
| What you observe | What it usually means | First thing to change |
|---|---|---|
| Fine dust, not chips | Chipload far too low. The bit is rubbing. | Feed faster, or lower the RPM |
| Brown or black edges | Heat from rubbing or recutting chips | See burning |
| Small curled chips, bit stays coolish | You are in the right area | Nothing. Note the settings down. |
| Loud rattling or a growl that changes pitch | Chatter: too much engagement, or something is loose | See chatter |
| Machine visibly flexing or the gantry shifting | Cut is beyond what the frame can hold | Reduce depth per pass first, then stepover |
| A grinding or screeching noise | Stop now. Dull bit, or the tool is buried and not clearing. | Stop, inspect the bit and the cut |
The order to back off when something is wrong
When a cut is not working and you are not sure why, reduce in this order. Each step costs you less than the one after it:
- Depth per pass. Cheapest fix, biggest effect on load.
- Stepover, if the tool is heavily engaged sideways.
- Feed rate, but only after checking the chipload, because slowing the feed makes rubbing problems worse, not better.
- RPM, usually downward, if you are burning and cannot feed faster.
The reflex that causes the most damage
When something sounds bad, the instinct is to slow the feed rate down. If the problem was heat, that makes it worse: a slower feed with the same RPM means thinner chips, more rubbing and more heat. Slow the spindle instead, or feed faster, and reduce the depth.