CNC Experiments: Baltic Birch Plywood

I’m planning some projects involving CNCing shapes from plywood and wanted to get a better sense of what tools/feedrates/etc will produce the best results. There’s a near-infinite supply of anecdotal feeds & speeds advice online, but not nearly as much data from controlled tests.

I recently bought some new end mills and was doing some test cuts of my own, and figured the results might be helpful for others.

TL;DR

To cut parts from Baltic birch plywood, use a 1/4” 2-flute straight end mill at 10k RPM and a feed rate of 150-200 IPM. Use conventional milling and a max pass depth of 0.25”.

The setup

Material: 12mm (measured 0.470”) Baltic Birch plywood

Tools: Two brand new 2-flute 1/4” end mills:

  • Freud 04-110 1/4” straight
  • Freud 76-102 1/4” down spiral

CNC: 48x96 inch ShopBot PRS at Pumping Station: One

I modeled a small test shape in Fusion 360 and generated sevaral toolpaths with varying feed rate, number of depth passes, and milling direction. Spindle speed was a constant 10k RPM.

Fig 1: Fusion 360 model and toolpaths

Here are the 8 samples I cut:

SampleToolFeed rate (IPM)PassesMilling direction
A1Straight752Conventional
A2Straight1502Conventional
A3Straight2252Conventional
A4Straight1501Conventional
B1Downcut1502Climb
B2Downcut1502Conventional
B3Downcut2252Conventional
B4Downcut1501Conventional

Results

I swapped the slowest cut (A1) for medium-speed climb cut (B1) when I switched from the straight to the downcut bit. I originally planned to redo all 4 parts as climb cuts, but decided to just do one for comparison as I knew conventional was better for my purposes (more on that later).

Straight vs. Downcut

The side walls of the downcut cuts had subtle ridges, while the straight tool’s cuts were almost perfectly smooth. The downcut was louder when cutting, and I assume those two things are related. The shaft of the downcut bit is about 1/4” shorter than the straight bit, so it’s possible the collet didn’t get as good of a grip on the downcut, causing some chatter. Not sure what else could have caused it, I certainly didn’t expect such a difference in finish between two such similar tools.

Fig 2: Downcut parts. From top: B4, B2, B3
Fig 3: Straight flute parts. From top: A4, A2, A3

The straight flute parts had a slightly cleaner bottom surface, which is expected, but the difference was very minor. I wouldn’t consider the difference to be significant, and would probably disappear entirely with light sanding (I didn’t sand at all before these photos).

Feed rate

I varied the feed rate from a definitely-too-low 75 IPM (0.00375” chip load) to 225 IPM (0.01125” chip load). The ShopBot can comfortably go a little faster, but I stopped there because with such a small part, it would have been unlikely to ever accelerate much faster than that.

There was very little difference in cut quality over this 300% variation in speed. The slowest cuts were slightly louder than the others, and the chips produced were noticably smaller, but nothing too concerning. One of the biggest effects of changing feed rate is the lifetime of the tool, so perhaps there would be a noticeable difference in that regard between 150 and 225 IPM. But for hobbyist-level usage, I’d be comfortable recommending anything in that range.

I’d like to test even higher chip loads by reducing spindle speed below 10,000 RPM, but that will need to wait for the next round of experiments.

Climb vs. conventional milling & other dimensional variations

I’ve noticed that climb toolpaths tend to produce parts slightly larger than their specified dimensions, and conventional toolpaths are usually right on. I think this is because of the deflection of the bit from the difference in force between the two sides of the path.

On each part, I used calipers to measure the width of the two “teeth”:

Cut typeMin (inches)Max (inches)Count
As designed0.9400.940-
Conventional 2-pass0.9370.94110
Climb 2-pass0.9500.9512
Conventional 1-pass0.9290.9314

The climb cut was about 0.01” oversized, and the 1-pass conventional cut was about 0.01” undersized. Precise dimensioning in wood is always an uphill battle due to heat- and humidity-related expansion, but these 0.01” variations make a big difference for joinery.

The long slots on each part were designed to be as wide as the thickness of the material (0.470”) to allow two parts to slot into each other. The smaller 1-pass parts could slide into each other easily, with some wiggle when joined. The conventional 2-pass parts could be joined with some force, but were difficult to re-separate. The climb-milled parts were too big (resulting in a slot too narrow) to be joined at all.

Fig 4: Straight bit parts with dimensions
Fig 5: Downcut bit parts with dimensions

Pass depth/number of passes

The A4 and B4 tests cut a single ~0.5” deep pass instead of splitting the depth into two passes. It sounded like the spindle was struggling a little more than with the other cuts, but the quality of the finish was still great. In fact, some of the 2-pass parts had a visible line halfway through the part at the bottom of the first pass (see Figure 3 above), so the single pass actually had a better finish.

The different sound when cutting, combined with the smaller finished dimension, leads me to believe that cutting 1/2” deep is causing excess vibration in the tool. If you’re really in a hurry it works well enough, but I’d advise going a little faster and taking two passes instead.

Conclusion

These tests didn’t cover the full range of every CNC parameter I’m interested in, but I definitely learned a lot by this more scientific approach. Hopefully others will find these observations useful as well!