X-Carve Milling Aluminum

Hi all,

I’ve been trying a new toolpath strategy on our shop X-Carve for a little while now. Yesterday I used it to produce a part from 6061 aluminum.

I figured I’d share my success here and outline how I created the toolpaths.

I used Inventor HSM to generate the toolpaths, but Fusion 360 will do the exact same thing and is completely free to hobbyists.

I started by adding tabs and surrounding material in the CAD model.

Then I switched over to the CAM section and selected 2D adaptive milling. This is a toolpath strategy developed by Autodesk that utilizes trochoidal milling techniques. From what I understand it attempts to keep a consistent load on the tool by keeping tool engagement consistent. In other words, if the first pass of your job seems OK the rest of it will probably be OK too. I was able to take much deeper passes with this strategy and increase my material removal rate by about 10 times over traditional toolpaths.

I made separate toolpaths for the large circular pocket, small circular pocket and cutout. The important settings were:

Feedrate = 40 in/min
Optimal Load = 0.5mm
Maximum Roughing Stepdown = 0.5mm

Then I made a “Bore” toolpath for the mounting hole. I used the default settings but changed the pitch to 0.5mm.

I used the grbl post processor that Autodesk provides to produce the G-Code.

Overall the job took a little less than 4 hours. The finish is pretty good, especially the bottom surface of the pockets. I used a cheapo air pump from our laser cutter to blast chips away and a small squeeze bottle to apply cutting fluid to the workpiece.

You can see a video of the job here:

Here’s the part after peeling away the “onion skin”, sanding away the tabs and using our deburring tool to clean up the bottom edge.

Here are some things I will try on the next attempt:

  1. Add finishing passes for the vertical walls
  2. Reduce the pitch in the bore operation
  3. Extend the cutout and small pocket depths to get rid of the “onion skin” and cut the part out cleanly

What spindle are you using? That is basically 1000mm/min and .5mm cut depth. You can see from my thread that about 125mm/min and .15mm cut depth is what I can do with the standard x-carve spindle. When I accidentally put in .4mm, it was not happy… (First attempt at aluminium milling)

I used our Quiet Cut spindle for this job. It’s really the toolpaths that make the difference, I used a helical ramping entry that gently eases the tool into the material and allows for much greater depth of cut and feed rate.

That’s incredible @TaitLeswing nice job.

So I think I have solved most of the issues I’m having with aluminum. The Y axis is no longer a problem. I also tried replacing the two flute Kyocera spiral endmill with a three flute SGS endmill made for cutting aluminum. I’m not ready to try Leswing’s crazy feed rates, but I did modify my tool paths to ramp into the material rather than plunging. This time around I only had two minor issues.

You can see the part came out nicely, and the edge finish is pretty good.

The corners of the pockets had some issues, especially this one. This isn’t the corner where the bit entered or left the pocket, so I don’t know what is special about it.

and here where it started the profile cut, the bit started chattering and deflecting. I think the anodization layer is much harder than the rest of the metal, so the cutter has a hard time with it.

@ChrisWundram what kind of tool path strategy were you using? Note that @TaitLeswing used:

With that strategy getting the right speed is important to make sure the bit is engaged. If it is too slow you will get rubbing and too fast you will break the bit. Tait did a lot of experimentation to get it to work. We are very much in the learning phase with these advanced tool path strategies but encouraged by the results you can achieve with an X-Carve.

This is just a conventional milling strategy. It spirals into each cut rather than plunging directly, but it mills slots straight ahead. For the outer profile I had it cut a wider slot with a stepover, which kept the part clean even with the trouble it had initially.

I was impressed with my results using Easle stock settings for aluminum! I used this single flute spiral upcut bit: https://www.inventables.com/technologies/solid-carbide-single-flute-upcut-end-mill-10-pack

I actually changed to a brand new bit a couple minutes into the job, because I was getting some chattering. After the new sharp bit went in it was beautiful. Examining the bits closer, I could see a little tang right at the tip that comes out a tiny bit wider than the rest of the bit. On my old bit this was worn down or broken from some earlier experimentation. I would imagine this wider tip would provide some clearance so the bit isn’t rubbing the sides when you get deeper into the material.


Was this with the Dewalt 611? If so, what speed setting did you use?

Nope, this was with the original X-Carve spindle.

1 Like