First Aluminum Part :)

Hey guys,

Just thought I’d share my very first aluminum part made with my 1,000 mm X-Carve a couple of weekends ago. Although there is definitely room for improvement (there always is), the results were better than I expected :smile:.

This is just a simple prototype part that I designed at work using Creo Parametric. The part model was then converted to “sketched” geometry using my own copy of TurboCAD at home. The sketched geometry was then saved as an SVG file and loaded into Easel to create the tool paths. We needed the part made quickly and I had just stiffened up my X-Carve’s X and Y axes, so I figured it was the perfect opportunity to try aluminum on my X-Carve. I’m so glad I finally went for it! Below are some pictures for your reference.


Milling complete:

And here is the finished fully functional part after some light sanding and tapping of the threads:

Now I am confident that my machine can mill aluminum :relieved:. I can’t wait for an excuse to mill out more aluminum parts!!

Question: do you guys know if there is a way to tell Easel to conventional mill the aluminum instead of climb mill?

Unfortunately, this part was milled entirely with climb milling. I would be interested in seeing how the side finish compares with conventional milling.



what kinda tool are you using?

I used a 1/8" single flute titanium nitride coated carbide bit that @ErikJenkins recommended at some point:


1 Like

yeah there are alot of tooling marks on that piece for sure

using the single flute bit is what you want I just personally hate the chinese tools in the long run I think that you will find that x10 bits for 20 bucks will not save you money

might look into Onsrud tools if you want quailty but you will pay for them but they will produce good results.

That beign said I do not think that the surface finish was only caused by the tool in this case

can you line out all of your specs that you used on the job including:

depth of cut
coolant method
and toolpath used I believe you said you were using easel and imo easel is not a great program for milling aluminum
the best way I have found to mill aluminum on a cnc router is to cut conventional but leave .020" and then go back climb milling and mill to final dimension this at least on my machines leave a great surface finish

also have you done any mods to your X-carve to give it any strength and reduce the flex?

also when milling aluminum try and use positive stops in addition to clamps this will help keep the piece extremely solid and not moving

I agree, the finish isn’t the prettiest… but it smoothed out fairly well after some sanding. It feels better in your hand than it looks in the pictures. It would be nice if I didn’t have to sand it though.

These were my settings:
• RPM ≈ 16,000 (setting 1 on Dewalt 611)
• Feedrate = 30 IPM for the top planing operation. Dropped to 25 IPM for step down, center hole and outline tool paths.
• DOC = 0.010" for planing, center hole and stepped feature. 0.005" for the outline (slotting).
• Stepover = 30%
• Coolant = None… other than air moved by my vacuum… don’t want to ruin my MDF.
• Toolpath/CAM = Easel

Here are the 2 stiffening mods I did to my X-Carve, specifically to start milling aluminum:

I will look into making some side stoppers next to hold the parts. I can see it helping hold things more securely.

I agree that Easel’s limits do become obvious when milling aluminum. There was definitely some chatter going on during the climb milling tool paths. The straight down plunges didn’t sound all that great either. Need to slow down my plunge rate. For these reasons, I am in the process of learning the CAM side of Fusion 360. Hopefully it will allow me to zig zag my plunges as well as do roughing and finishing passes as you describe.

Do you recommend sticking with single flute Onsurd tools? Or 2 flute using our CNC routers? TiN coated?

Let me know what you (and others experienced with aluminum) think about my settings. I’ll take all the advice I can get!


While not on an X-carve I mill a fair bit of aluminium and proper end mill is the main factor besides speed/cut rates.
I have some cheap and generic 2F upcut that I feel are very rough, also 3F upcut that are very rough aswell.

My favourite bit by far is this one:
While consensus say 1F is better this it a 3F upcut bit it work very well for me, very smooth cut and also very quiet (which I think is a good indicator)
Longest continous run I have done with it is 3hrs and I have probably accumulated 20hrs of machine time on one bit alone. (also broken one and gummed up a couple but that was due to machine error/flex/user initiated oopsies)

My run data is:
RPM 10k (Makita RT0700 at setting 1)
Feed rate around 60inches/minute
DOC 0.004"
Stepover (40%, Easel default)
Plunge 3inch/minute
Aluminium stock/end mill/router is almost cold to the touch, no sign of heat.

My diy-machine is not rigid enough yet to go faster/more aggressive DOC. Due to this I also leave some material for a finishing pass which I run with slower feed rate/deeper DOC.

With the Dewalt minimum speed setting you should in theory do 95"/min with the same chip size as I am at.
I have not played with Onsrud or other quality end mills.