Baltic Birch Ply Cut Failure - chipload help

1

Hey there! Pretty new to my Onefinity Elite Journeyman (w/stiffy and Makita 0701). I’m cutting some 3/4" baltic birch ply, and trying to figure out what feeds/speeds I can reliably use.

TLDR: machine cut wavy lines and then bogged down & stalled at 200ipm, 5mm pass depth, 12000RPM, 2-flute compression bit. Test cuts at those settings seemed to work fine. But when I made my first “trial production” cut with those settings it started wandering badly during the second pass, making a ton of noise, and eventually the router stalled and the Onefinity stopped with with an x-axis motor fault.

I’d like advice on what may have gone wrong, and which direction to take my experiments to efficiently find the feeds & speeds I can safely use. Was it more likely the router torque not keeping up? The machine insufficiently stiff? Pictures follow.

Fuller explanation:
This 1/4" 2-flute compression bit is nearly new (like 15 minutes of use).
I did a few test cuts at 300ipm with passes at 7mm depth, setting 3 on the Makita (18000RPM). That should be 0.009" chipload if my math is right. I had the depth just below the upcut portion of the bit to reduce tearout.

Those settings cut but were pretty loud, and I noticed some curvature on surfaces for the first couple inches after making a 90 degree turn - definitely not straight lines.

I figured either the bit or the machine was deflecting, so I decided to be less aggressive. I switched to 200ipm, 5mm depth, setting 2 (~12000) on the Makita. That should be 0.008" chipload. 5mm doesn’t get the upcut portion of the bit into the material, but I added a 0.5mm full-depth finish pass at 100ipm and the results seemed good in my test cuts. The test cuts were producing reasonable sized chips instead of fine dust and everything seemed okay.

So I transferred those settings to the first full “production” cut of parts I cared about, loaded a quarter sheet of plywood, and let it rip. The first pass looked great so I stepped away to tidy up the shop. About a minute later I started hearing a noise that definitely didn’t sound right. By the time I ran over to the machine, the router had stalled and the job halted with an x-motor error. It had cut wavy lines around a large portion of the perimeter, but that didn’t start until the 2nd pass.

Advice on which direction I should modify my settings to start getting reliable cuts would be greatly appreciated.

Picture notes: before doing this perimeter through-cut, I’d done some pockets, mortises, and holes with a 1/8" downcut 2-flute bit, so you’ll see those in the pictures. I had run those at 375ipm, 27000 rpm, and they seemed to work fine. I’ve included a couple screengrabs of what the paths look like in Fusion.

Fusion360_EP4P7XCxNd
Fusion360_EP4P7XCxNd1227×670 147 KB

Fusion360_D8er1JvfSW
Fusion360_D8er1JvfSW1386×809 218 KB

PXL_20241114_011520638
PXL_20241114_0115206381920×2550 193 KB

PXL_20241114_011904383
PXL_20241114_0119043831920×2550 248 KB

PXL_20241114_011907965
PXL_20241114_0119079651920×1446 186 KB

2

Have you tried slowing down ? You may be asking to much of your router.

The pockets you cut look ok. What recipe did you cut those ?

How is the material secured ?

1 Like
3

Is the router secured properly, any play anywhere?
To me that seems a little fast

4

Evan,

Since you have an elite (Masso), I recommend running in manual override for feed rate. You can dial back the feed rate on the fly until you get the desired smooth pass going. Maybe set your file to about 200 ipm, and then once plunged in, slow the feed rate down until you hit a sweet spot (no deflection) of the bit. I also wouldn’t use a Makita turning that slowly, go no less than 18,000 or more like 21,000 for the motor setting. At 12000, your probably only getting about 1/2 horsepower from that little guy, and that will kill it pretty fast, not to mention vibrating like crazy. Also our local lumber companies have 2 different plywoods, a light weight and a dense version that weighs nearly double. The light weight called sandeply will chip out at any chipload above .006, so I limit myself to that.

Looking at your pictures, I’d say you’re pushing too hard on feed / depth and the slow rpm are causing the Makita fits, the runout on the bearings for that router are usually horrible. If you want to cut that aggressively, you need a spindle. I have a 2.2 Kw water cooled and I don’t usually run it more that 200 ipm at 1/4" depth and its putting out about 3 - 3.25 Hp at 20,000 rpm.

1 Like
5 
Have you tried slowing down ? You may be asking to much of your router.

As mentioned in the post, this was already slow-down from my previous test cuts, but maybe not enough. So that’s what I’ll try next. I think my main question is: is it more likely that I’m pushing the router too hard, or pushing the onefinity too hard? I’m leaning towards the router.

The pockets you cut look ok. What recipe did you cut those ?

The pockets were cut with a 1/8 downcut bit, at higher speeds: 375ipm. They’re also mostly pretty shallow. So, higher speeds but much less load on the router because of the smaller bit.

How is the material secured ?

It’s screwed to the wasteboard with brass woodscrews.

I own some of the “oops clamps” that onefinity sells but I found them to be slow to set up, fiddly to use, and don’t always hold well enough for high load operations on hard materials like Baltic Birch ply.

6

The router seems pretty secure, but at the very end when it stalled and got bound in the wood, it did twist in the mounting by a few degrees.

Right now it’s the stock 80mm mount from onefinity, with a 3d-printed spacer/adapter to hold the 65mm router.

7 
I also wouldn’t use a Makita turning that slowly, go no less than 18,000 or more like 21,000 for the motor setting. At 12000, your probably only getting about 1/2 horsepower from that little guy, and that will kill it pretty fast, not to mention vibrating like crazy.

Okay - that makes sense, but leave me concerned about chipload.

If I bump the speed to #4 (22000 RPM on a Makita) and slow the feedrate to 150ipm, say, that would give me a chipload of only 0.003. Which I have read elsewhere is way too low. Every CNC youtube video everywhere says if you run the operation with too low a chipload, you’ll overheat and burn out the bit.

That’s in part why I’ve been running my feeds so fast, is to get the chipload into a recommended range for hardwood. (0.009"-0.011" chipload for a 1/4" bit)

I am considering this a sacrificial bit, to learn and make mistakes on. Once I figure out what I want to do and a set of feeds-n-speeds I can rely on, I’m going to replace it with a couple higher quality coated carbide bits.

8

The speeds and feeds that high-end bit manufacturers recommend are typically geared toward industrial CNC’s, which are much more rigid than a Onefinity. Personally, I’ve had good results machining BB ply with a Makita at a chip load of about 0.005".

Looking at your ragged cuts, I strongly suspect that the router is resonating side-side as it cuts. The “envelope” of the cut is fairly symmetrical, but the lateral amplitude of the resonance varies as the bit travels along the cut.

This is pure speculation, but the 3D printed adapter could be part of the stiffness problem. I purchased one of them myself when I bought an Elite upgrade, so that I could shake things out before installing my new spindle. But the adapter was suspiciously lightweight, as if printed with very low infill. And then when I installed it, the Onefinity spindle mount compressed the adapter considerably. So I decided bail on that, and go straight to using the new spindle. The fact that your router rotated in the adapter further increases my suspicion. If I do ever want to install my Makita on the machine again, I’ll print a good solid adapter ring myself.

2 Likes
9

That is a great observation. I never thought of the adapter ring being a part of the problem when i have issues. Making me check mine now.

1 Like
10

Thanks for the tips.

I did in fact print this apadpter myself, With (IIRC) 8-layer-deep walls with 75% infill in cubic pattern. Maybe I’ll go back and just print one with 100% infill and see if that helps.

In the meantime, I’ll try reducing my chipload and going slower speeds to see if I can get satisfactory results.

I do plan on upgrading to a spindle soon, but it’s a time trade-off. I’ve spent SOO much time this year upgrading my shop and not enough time marketing and selling.

2 Likes
11

I cut 3/4” Baltic Birch from time to time
For me the Makita router is for light pass cutting 18000 and 50 ipm seems to be the max imo
Anything faster would cause the bit to loosen in the collet causing it to drop
When I get a spindle then maybe 100ipm but not with a trim router