That'll buff out

This used to be a ¼" O-flute carbide up mill, until I tried to route aluminum with it in my OX. 18600 RPM, .2mm DOC, plunge 60mm/m, feed 600mm/m, made a little noise but I convinced myself that it was ok until the excess compliance in the router let the tip bite in just a little bit too much, and then I was glad I was wearing polycarbonate goggles.

A little super glue and I’m sure I’ll be back running in no time! :wink: :rofl:


Next try will involve ball-end HSS mills that arrive this week. I’m getting some 4mm and 6mm ball mills with enough cutting depth for this part.

The good news is that until the tip snagged, more than half an inch deep into the part I was cutting, the pocket was clear of chips, so air assist was working well.

1 Like

Just out of curiosity, what spindle are you running? The quiet cut spindle I bought with my Ox only goes to 10K RPM.

I’m using a 1.5kW water-cooled brushless spindle with a VFD. That would probably be a bad idea on an otherwise stock OX, so I’m using a C-beam gantry, everyman double belts, and I’m lifting Z with a single-start lead screw in an anti-backlash nut. The plates to support this configuration are at Michael K Johnson / C-Beam OX · GitLab


Are these the ones you “posted” on Twitter the other day? :wink:


I used the wrong paste buffer. I’m on Linux, so I have both control-c/control-v and middle mouse button paste, and I use both. Sometimes it bites me.


Required new gcode for ball-end mills. Put the 6mm ball mill in and started it going. Seemed to be working fine. But suddenly it made noise and wasn’t following the edges properly. Hit the e-stop. Candle showed it in the second cut but the mill was in the first.

Careful investigation showed that my new diaphragm Z coupling was slipping on the lead screw. In retrospect, I’ll bet this is what happened that shattered the first bit. This time the bit was OK, other than some BUE that was a pain to remove. Ended up sliding a razor blade behind the aluminum (not against the cutting edge of the mill) to pop it off.

So I cleaned things up with acetone, added thread lock, and re-assembled it. Now waiting for it to cure. I guess I should wait 24 hours for a full cure before running it again, because if it fails I’ll be really annoyed.


It’s hard waiting 24 hours on the weekend, but — that’s working better! My air assist tangled with the collet nut, so I removed it; the vacuum seems to create enough turbulence to evacuate the chips from the holes so far.

I’m finally getting to the benefits of this OX upgrade. Cutting a somewhat gummy cast aluminum plate successfully (so far!) is :tada:

Here’s the start of my first test cut:

By contrast, here’s the cut where the bit was stuck in the hole due to slipping Z:


There’s still a bit of noise; 19mm plate requires a mill with plenty of cutting length, so it’s a bit flexible and sometimes sings a bit, but not too bad. And the edges look clean.


It was looking so good with the 6mm ball mill.

The 4mm ball mill was less of a success, and slowing down feed radically wasn’t enough to resolve the issue.

So now I’m pondering what to do next. I hate the idea of moving to the mill, where I have about 1/10 the RPM available… but it’s a lot more rigid, and I have enough travel for this part.


I am late to the party here, but are you ramping in? I cut aluminum with my (based on the Ox) CNC router. I cut 0.8mm deep at 900mm/min at about 18000rpms with a 1/4" 2 flute endmill and get a great finish. I ramp in all my cuts. For holes I spiral cut. I leave about 0.2-0.3mm for a finishing pass. Although I have never used a ball end mill in aluminum, in wood I cut much faster with one than with a regular endmill.

1 Like

Thanks for chiming in!

I am using kiri:moto to toolpath, and as far as I can tell it doesn’t have spiral cut. I had thought that “ease down” was ramping in but I think not. [Update: it is intended to be ramp in but is not fully implemented at this time.]

My first try was to clear the voids with a 6mm ball end (24000 RPM, 1600mm/minute) and then take another pass with a 4mm ball end (24000 RPM, 1400 mm/minute) intending to get the corners of the pockets (as shown above the outline in the picture) but it was starting to chatter going into those pockets, so I turned the feed way down to 20% so 280 mm/minute. That was when it started wandering while cutting the outside and I hit pause.

The sides have a 2.2° draft angle, so a ball mill seems necessary to avoid a stepped finish. But now that I understand (I think) why the carbide bit exploded, maybe I should get a 4mm 2-flute flat endmill to rough, and use a 4mm ball mill to finish, so I don’t have those pockets. With that I might even be able to rescue this part. (The wandering section isn’t a big deal.)

1 Like

I’ll try roughing with a 4mm end mill and finishing with a 4mm ball and :crossed_fingers:

I just had to order 4mm end mills with enough cutting length for this application.


That plan sounds like the way to go. I really need to try 3D carving in aluminum. I have been very successful at plate cutting, but I have a few molds in mind I want to make. Maybe then I can offer better advice. I just got a shipment of ball end mills in from Kodiak Cutting Tools. I needed a 100mm long 1/8" for a finishing pass on a 3D carve on some 3 inch thick stock and shipping is free when you break the $100 mark so I put in a few other sizes as well. Surprisingly the made in America Kodiak 1/8" extra long ball end mills were the same price as a 3mm I ordered (and broke) from China.


Thanks for the tip on Kodiak! That may put more pressure on my search for good Tool crib numbering systems so I can have a sane and consistent scheme between different CAM tools. :relaxed:

Just curious, what kind of molds are you looking at making?

Looking back, I see that I was feeding harder than you do. I had a shallower DOC (0.3mm) but equivalent chip load at 24000 RPM would be 1200mm/min for a ¼" and slightly less for the 6mm, where I was running 1600. I wonder if the small DOC let the ball mill ride up instead of cutting when it ran over an edge. I’ll still finish with a small DOC for the draft, but roughing with more depth might make sense. (Kiri:moto not having ramp-in fully implemented might limit the DOC I should use there; I’ve asked about that on the kiri:moto discord.)

Update: tonight’s kiri:moto development update has updates to improve ease-down (ramp-in)!

1 Like

I will be curious to see your results. As I said, I have only cut 2.5D stuff like aluminum plates to upgrade the existing CNC and for my recent CNC lathe build. Now I need to start on some plates to upgrade my K40 and make a rotary axis.

As for the molds I am making, they are for making larger lead sinkers for salmon fishing. I have molds or 8 and 10 0z, but I need some 14s and 16s. I found some 1 inch thick scrap pieces I will try it with when I get a chance. Premade molds that large are hard to come by and are expensive in those sizes. I cast a 12 oz lead ball in plaster of paris and made a two part mold. But I underestimated the needed drying time. For the short time it existed, it successfully made one 12 oz sinker and then abruptly and semi-violently released the trapped water vapor. If you ain’t failing, you ain’t learning.

1 Like

These cheap 4mm end mills don’t come with any specs and I’m cutting mystery metal so it’s all trial and error. 0.6mm DOC and 1200mm/min filled the flutes with BUE and snapped the mill.

Here’s where it broke:

Look at all that BUE clogging the tip!

Trying again running the same gcode, but with feed at 50% in Candle.

If that breaks, I can reduce DOC.

It’s quite possible that this stuff is just so gummy that it’s hard to cut well without coolant/lubricant, which would mean the OX is even more the wrong tool. :relaxed:

1 Like

50% feed snapped another mill when I tried it.

I toolpathed again with latest kiri:moto with more ease-down/ramp-in implemented. I’m doing two passes:

  • Roughing: 0.2mm step-down, leave .2mm stock, 600 mm/min feed, 200 mm/min plunge, 4mm end mill — that’s an absurdly small 5 tenths of chipload. It’s making dust. But that might be what I need with these long flexible mills (22mm cutting length in a 45mm tool, cutting down to 19.1mm.
  • Outline: 0.3mm step-down, 500 mm/min feed, 200 mm/min plunge, 4mm ball mill

I also worked up a better air assist that doesn’t interfere with the dust boot; it’s superglued to the rear gantry plate and I’m using real loc-line because it is easier to position more precisely than the knock-off I was previously using. The block is from a broken mist coolant and I just removed the coolant line because I’m not using coolant on the OX; it would mess up both my spoil board and my dust collection.

The roughing pass is maybe ⅓ of the way through and I think this stands a chance of being better. :crossed_fingers:


I think the air assist was an improvement.

I don’t know if it’s the 9-year-old laptop I’m using, the MKS control board, the 10-foot long USB cable, or something else, but the control board crashed when I was about a millimeter short of finishing the roughing pass, and my X/Y 0 registration wasn’t good enough to follow to get back my zero and start over. But at 0.2mm step-down, the part wasn’t too rough to use.

I used double-stick spectape to tape the front down to a piece of MDF to hold it together (thanks again @donkjr for the recommendation) and used a face mill on my bench mill to take a couple mm off the back. I was very careful not to trust the tape too much, but when it finally came time to remove the part, I needn’t have worried. I ended up having to use the vice to remove the part from the tape it was stuck so well!

1 Like