Chip Chad
Set your feed rate in CAM and you have a number that means almost nothing by itself. It depends on your spindle speed, how many flutes are on your cutter, and what material you're cutting. Chip load is the number that actually tells you what the tool is experiencing, and it's what separates a clean cut from a rubbing mess.
What chip load actually is
Chip load is feed per tooth: the thickness of material each cutting edge removes per revolution. The formula is simple:
chip load = feed rate ÷ (RPM × flute count)
At 18,000 RPM with a 3-flute end mill running 86 IPM (2185 mm/min):
86 ÷ (18,000 × 3) = 0.0016 in/tooth (0.041 mm/tooth)
That 0.0016" (0.041 mm) is what the edge actually sees. The feed rate and the RPM alone don't tell you much. The chip load tells you everything.
Why chip load matters more than feed rate
Two setups can have identical feed rates and produce completely different results.
- Same feed rate, fewer flutes = higher chip load per tooth. A 2-flute cutter at 86 IPM and 18,000 RPM sees 0.0024" (0.061 mm) per tooth instead of 0.0016" (0.041 mm) — a 50% increase in load.
- Same feed rate, lower RPM = higher chip load. Drop to 12,000 RPM and chip load climbs to 0.0024" (0.061 mm) regardless of flute count.
Feed rate is the output. Chip load is the input you actually control.
Chip load ranges by material
These ranges reflect two realities: what's published for the tool under ideal conditions, and what actually works on a hobby machine.
| Material | Published ideal | Hobby machine starting point |
|---|---|---|
| 6061 aluminum | 0.001–0.005" (0.025–0.127 mm) | 0.001–0.002" (0.025–0.051 mm) |
| Mild steel (1018) | 0.001–0.004" (0.025–0.102 mm) | 0.0005–0.001" (0.013–0.025 mm) |
| Hardened steel | 0.0005–0.002" (0.013–0.051 mm) | 0.0003–0.0008" (0.008–0.020 mm) |
| Wood / plywood | 0.003–0.010" (0.076–0.254 mm) | 0.002–0.006" (0.051–0.152 mm) |
| Plastics (acrylic, HDPE) | 0.002–0.006" (0.051–0.152 mm) | 0.001–0.003" (0.025–0.076 mm) |
The gap between published and hobby starting points exists because published values assume a rigid machine with minimal deflection. Hobby routers and benchtop mills flex. Start at the low end of the hobby column, listen to the cut, and work up. A good cut sounds like a consistent hum.
Plastics deserve a special call-out: they melt at low chip load. If you're cutting acrylic and getting a gummy, melted edge, you're not cutting hard enough. The fix is to increase feed rate, not reduce it.
Too low: the rubbing problem
Below the tool's minimum chip load, you stop cutting and start rubbing. The edge deflects over the material instead of shearing through it. The consequences:
- Heat — friction instead of chip formation. Heat goes into the tool and the workpiece, not the chip where it belongs.
- Work hardening — especially bad with stainless and titanium. The surface you've rubbed is now harder than the stock you started with.
- Premature wear — flank wear accelerates dramatically at low chip loads. You'll blow through tools faster running light than running hard.
The symptoms are recognizable: dust-sized chips instead of curls, discolored or blue-tinted chips, a hum that gradually shifts pitch, and edge chipping that starts earlier than it should.
Too high: the overload problem
Above the tool's safe chip load, you're asking the edge to take more than it can handle. At moderate overload you get deflection and chatter. At severe overload you get instant breakage.
Signs you've pushed too far: a squealing cut, visible flex in the part or tool, chipped corners on the flutes, and finish that looks like corduroy.
Understanding radial and axial engagement
Before explaining chip thinning, two terms worth knowing — because your CAM software uses them constantly.
Radial engagement (WOC — width of cut) is how much of the tool's side is in contact with the material. Think of a wheel spoke extending outward from the hub: radial = outward from the center = the side of the cutter = stepover. Full-slot milling is 100% radial engagement. A light finishing pass along a wall might be 5–10%.
Axial engagement (DOC — depth of cut) is how deep the tool is cutting, measured along the tool's axis of rotation — straight down in a vertical setup. Think of the axle of that wheel: axial = along the axis = depth.
In short: radial = the side of the cutter, axial = the depth. When Fusion 360 asks for "radial depth of cut," it wants your stepover.
Chip thinning: when chip load isn't what you think
At low radial engagement — WOC below about 50% of tool diameter — the actual chip formed is thinner than your programmed chip load implies. The tool meets the material at a shallower angle, so each tooth takes a thinner bite than the formula suggests. This is called chip thinning.
The precise relationship:
adjusted feed = target chip load × √(D ÷ (4 × WOC × (1 − WOC/D)))
Where D is tool diameter and WOC is the radial depth. At 10% engagement on a 1/4" (6 mm) tool, you need to program about 1.7× your target chip load to actually achieve it.
If that formula looks like a lot — it is. This is exactly what Chip Chad calculates for you. Set your WOC and target chip load; Chip Chad adjusts the feed rate automatically. You don't need to run the formula manually, but it's useful to understand why finishing passes and trochoidal toolpaths call for higher feed rates than roughing at the same chip load.
Putting it into practice
Start from the hobby machine column in the table above. From there, listen:
- Consistent hum, clean chips — good chip load, keep going
- Squealing, dust instead of chips — too light, increase feed
- Chattering, squeaking with visible flex — too heavy, reduce feed or DOC
- Rhythmic thump — something is loose, stop immediately
Once you're in the right range, Chip Chad keeps RPM, feed, and chip load coupled so adjusting one updates the others automatically.
Sources
- Sandvik Coromant, Entering angle and chip thickness in milling — documents the entering-angle modification factors and radial engagement adjustments: sandvik.coromant.com
- Dapra Corporation, Radial Chip Thinning — practical adjustment factors with worked examples that match the formula above: dapra.com