A stock X-Carve (1000mm) will cut Aluminum

I have a home built D-Bot CoreXY (300x200x325 print size) and a Prusa i3 (200x200x190 print size).

It takes ~15 minutes to print a clamp.

The quality of your printer will dictate your ‘visible layer’ lines. For example, my D-Bot produces far smoother parts with a higher level of detail than my Prusa (i could easily upgrade my Prusa to match my D-Bot… but i don’t see the need).

3D printed object can be incredibly strong and durable. It all depends on the type of filament used. I just use standard PLA for my x-carve clamps and they are stronger than any hardwood clamp i’ve used… and PLA wouldn’t be called a ‘strong’ filament.

PLA, ABS, PET, TPU, Nylon… and may other blends of plastics are available to print with (for example… 80% copper powder, 30% PLA = CopperFill http://learn.colorfabb.com/print-copperfill/).

what resolution do you normally print in?

I might be jaded by the prints that we get from the maker space http://ppld.org/c3/makerspaces.
We’re not allowed to operate the machines ourselves and submit jobs to be run.

90% of my prints are at .2mm. If it’s something for ‘show’ (desk toy) I’ll do .1mm… and very rarely do I go below that.

Here is a post i did about my latest printer…

definitely well said! I have been doing aluminum as well with the stock 1000 m x carve, cutting thick and thin aluminum, no lubrication, and even cutting 10’ x 2’ sheets of aluminum (tiling).

I just completed a youtube video that goes thru step by step to do aluminum with out lubrication. This starts from how to draw in autodesk fusion, assuming you know nothing about the process, so you may want to fast forward thru some.

This vid is a timelapse of cutting 3/16" aluminum without lubrication:

If you are interested in how I use the X carve to tile and cut one 10’ wide piece of aluminum, you can watch this video:

What a fantastic machine eh?


I have used the bit Brian talked about in the original post and it does a pretty good job cutting AL, but 1/8" bits flex a lot and I found going up in cutting diameter allows faster cutting rates. I bought this bit:

With the 1/8" bit I found that the bit flex would cause chattering before the CNC flex caused chattering. I could see that the bit motion was larger than the spindal motion when chattering. When I stepped up to the 3/16" bit I actually found that chatter was caused mostly by the CNC flex, but I was able to cut at a much faster rate. For reference I have the 1000mm setup with all the upgrades.

Going off memory I think I was using 10in/min, 0.08" cut depth, spindal speed near max, dry cutting. I tried wet cutting with lubricant, but I did not find it improved my cut rate significantly. The Amana bits are pricey, but I think they are worth it.


@BillWalter Thanks for the info… I’ve ordered that bit and will give it a try :slight_smile:

1 Like

Great info and your brackets look great.

I have a project brewing and ordered the bit you recommended. The feed rates you list are fantastic. Others have stated closer to 10 in/min. Do you think that is due to the style and type of bit or are they just more conservative.

I know your post is a few months old, anything new you’d add?

It’s funny you posted today… because i was cutting more brackets on that same aluminum sheet yesterday.

I still use those same settings (30 in/min & 0.005 in depth per pass) on 6061 aluminum. I found that on some tricky aluminum like ‘Cast Jig Plate’ (ATP5/Mic6) i have to go a little slower (~25 in/min) or i get some slight jittering. It might have to do with how gummy ATP5 is… but it still cut like butter.

That Kodiak bit is still going strong and working great :slight_smile:

^ Picture of the new bracket… and if you look in the background you can see the ATP5 1/4" build plate i cut a few weeks ago.


I have a client that wants to be cut some very thin aluminum…not sure what it’s composition is (6061??) it is used for a trophy shop plate. Anyway, its very thin about the thickness of 2 business cards.

What you suggest for cutting out a simple circle as far as speed and DOC.

Is your machine stock or modified(if modified, what mods). The defaults in easel work for a stock machine. You can up it from there if you have modifications. I have a modded machine and I run .005 at 50ipm(currently) with a 0-flute upcut. A 45deg helical bit would also work well.

So, modified machine or stock?


I just cut some 1/4" ATP5 for a large buildplate as well. I wish I had known the X-Carve was capable, I would have used it instead of taking it to a water jet!

Anyone know if similar feeds and speeds (30ipm at 0.005" depth of cut) can be used with the quiet cut spindle? I have a stock 1000mm X-Carve (the newer single extrusion gantry style). I think I will probably stiffen my y-axis a bit before I try cutting aluminum since that can be done fairly easily.

Hello Brian,

Thanks for sharing that info.
I tryed the same on a 6061 T6 Aluminum (0.0591 thick) and I ruined 2 router bits. I have a dewalt 611 on my x carve and I was running it on the speed number 6. The first inch or inch and half was cutting good and the you can see in the photo the results of my second sample.

Any idea?

Thank you.


I am going to assume the thickness is actually 0.591"
The router should have been set on 1 and a single flute works best.

1 Like

You really need to run some cutting oil on that. The part will cut cleaner, and will keep the aluminum from sticking to the cutter. Thread cutting oil is the best commonly available oil to use, but WD40 will also work.

Having the 611 set at 6 seems a little fast… I’m normally around ~3 with a single flute bit.

1 Like

Feedrate? Depth of cut?
For a slotting profile cut like that, you want feedrate to be high with a smaller depth of cut. If you can, avoid slotting.

Stepover 0.381 mm
Stepdown 0.127 mm
Feed rate 5 mm/sec
Plunge 5 mm/sec

I used this bit: Cnc bit: Kodiak #149560 1/8" carbide end mill ,2 flute, 1/2" loc x 1-1/2 OAL, 45deg for Aluminum, which it was mentioned by BrianM

Blockquote Get a good bit. This is what i use…

Speed on the router: # 6

1 Like

At that feed, you’ve got a chipload of about .005mm. That low and you’re basically rubbing the aluminum away. That’s why you saw the melting.
Increase that feed to about 1370mm/min (22.8mm/s) for a chipload close to 0.0254mm (0.001 inches) which is where you want to be to get decent chips.
Depth of cut really depends on the toolpath and the machine. Keep it shallow for slotting cuts. I’d recommend using Fusion 360 or another capable CAM program and setting up adaptive toolpaths.
If you decrease the speed to #3 (20400rpm), you’ll also want to decrease your feed by the same percentage (so, about 1036mm/min).

By the way, if you can’t get that melted aluminum out of the endmill, a soak in purple degreaser will take care of it.