CNC chipload chart: wood, MDF, plastic and aluminum
Chipload is the single number that decides whether a router bit cuts cleanly or burns, melts, chatters or snaps. It's the thickness of the chip each cutting edge takes on every revolution. Get it in the right range and the edge comes out clean, the bit stays cool and lasts. Get it wrong and no amount of fiddling with depth or bit brand will fix it.
The chart
These are starting ranges for solid-carbide spiral bits, in inches per tooth, from the CNC Router Store chipload chart. They assume a rigid machine. Treat them as a place to begin, then adjust from test cuts.
| Material | 1/8 in bit | 1/4 in bit | 3/8 in bit | 1/2 in bit |
|---|---|---|---|---|
| Softwood / plywood | 0.004–0.006 | 0.009–0.011 | 0.015–0.018 | 0.019–0.021 |
| Hardwood | 0.003–0.005 | 0.008–0.010 | 0.014–0.016 | 0.018–0.020 |
| MDF / particle board | 0.004–0.007 | 0.011–0.013 | 0.015–0.018 | 0.020–0.023 |
| Soft plastic (HDPE) | 0.003–0.005 | 0.007–0.010 | 0.010–0.012 | 0.012–0.016 |
| Hard plastic / acrylic | 0.002–0.004 | 0.006–0.009 | 0.008–0.010 | 0.010–0.012 |
| Aluminum (with lubricant) | 0.002–0.003 | 0.003–0.005 | 0.004–0.006 | — |
To convert to millimeters per tooth, multiply by 25.4. A 1/4 in bit in plywood at 0.009–0.011 in is about 0.23–0.28 mm.
The bit maker's own chart for your exact series always takes priority. Different flute geometries, coatings and compression bits have their own recommendations.
From chipload to feed rate
You don't type a chipload into the machine. You set spindle speed and feed rate, and chipload follows from them:
Feed rate = RPM × number of flutes × chipload
Example: a 2-flute 1/4 in bit in plywood, at 18,000 RPM and a chipload of 0.010 in: 18,000 × 2 × 0.010 = 360 in/min.
That's fast. Many hobby and desktop machines can't cut at 360 in/min with any rigidity. The chipload calculator runs the formula the other way: enter the feed and RPM you're actually using and it tells you what chipload you're getting and how it compares with the range.
Why slower isn't safer
The instinct when a cut looks rough is to slow the feed down. With the spindle still at full speed, that shrinks the chipload. Below a certain point, the bit stops slicing and starts rubbing. Rubbing makes heat:
- Wood scorches, leaving brown edges and a burnt smell.
- MDF turns to fine dust instead of chips, and the bit dulls quickly.
- Acrylic and HDPE melt and re-weld behind the bit, leaving gummy edges and sometimes wrapping around the bit.
- Aluminum chips can weld to the flutes, and the next pass breaks the bit.
Heat also kills bits. A dull bit rubs more, which makes more heat. It's a loop.
The fix on a machine that can't feed fast enough is to lower the RPM, not the chipload. At 12,000 RPM, the same 0.010 in chipload needs 240 in/min instead of 360. If that's still too fast for your machine, go lower on RPM, or use a single-flute bit, which halves the feed needed for the same chipload.
When to go above or below the chart
Go lower when:
- The machine is light or flexible (belt-driven desktop routers, long gantries).
- You're using a long bit with a lot of stick-out.
- You're cutting deep in one pass.
- You see chatter marks or the machine sounds strained.
Stay in range or go a little higher when:
- You're getting burning or dust instead of chips.
- Edges are glazed or melted.
- The machine is rigid and the cut sounds smooth.
Change one thing at a time and make test cuts in scrap.
Reading the chips
The quickest check is the waste in the dust shoe or on the table:
- Fine dust, warm bit: chipload too low.
- Clean, distinct chips, cool bit: about right.
- Large chunks, tearing, loud chatter, deflected edge: too high, or too deep a pass.
In plastics, you want small curls or flakes, not strings or melted blobs.
Depth of cut and stepover
Chipload is per revolution; depth of cut is how much the bit engages vertically. Common rules of thumb for profile cuts in wood are a depth per pass of around the bit diameter, less in hardwood and much less in plastics and aluminum. For pocketing, a stepover of roughly 40% of the bit diameter is a common starting point for roughing. Deep, full-width slots load the bit much harder than an edge cut, so reduce chipload or depth there.
Flutes and bit types
- 2-flute upcut/downcut spirals: the general-purpose choice for wood and MDF. Upcut clears chips and can fuzz the top face; downcut leaves a clean top edge but packs chips into the slot.
- Compression bits: upcut at the tip and downcut above, for clean edges on both faces of plywood and laminated sheet. They need the cut deep enough that the downcut section is engaged.
- Single-flute (O-flute): the usual choice for plastics and aluminum, because the large flute clears chips and keeps heat down.
Or let someone else dial it in
Getting feeds right takes test cuts, scrap, and a few broken bits along the way. If you'd rather skip that, post the job and let makers who cut your material routinely quote it. Posting is free, there's no buyer fee, and the payment is held until the parts arrive and you confirm delivery.