Cutting Aluminum for a Sign

Need some advice. I am attempting to cut some 8" letters for a sign out of 090 Aluminum that is just under 1/8" thick. First pass broke a bit almost instantly. I bought an amana bit for this project.

51503-Z Solid Carbide CNC Spiral ‘O’ Flute, Aluminum Cutting 1/8 Dia x 1/2 x 1/4 Shank Down-Cut ZrN Coated Router Bit

I ran the CNC at 30 ipm with a .03 depth of cut with the Makita router set on number 3.

Bit only ran a couple of inches and broke. No chips were created during this short run but did get long strands of aluminum sticking up.

I called the local Rockler to see if they had a replacement bit and the guy said to just run my regular 1/8 bit and that it would cut aluminum (Bits & Bits 1/8" Down-cut Spiral Astra Coated).

So I loaded it up and cut the feed rate down to 20 ipm with a .01 depth of cut thinking that I was cutting too fast and deep with the Amana bit. This worked but with mixed results. (See photos) Again, no chips were cut during this pass. It basically melted the aluminum. The sheet got so hot that it warped and left a molten trail of aluminum to the shape of the letter.

Can someone please give me some guidance on feed rates and depths of cuts and RPMs? I am new to CNCs and afraid that I bit off more than I can chew with this one.

Cut your feed rate and plunge rate down to 5, your depth of cut to .015, your router down to a speed of 2. I’ve never cut aluminum, but that’s what I use with brass and copper and don’t have a problem. I also glue the sheets to mdf with hide glue so there is no flex. You can remove the pieces with a heat gun afterwards or soak them in water overnight.


I’ve found milling brass nicer than Aluminium: not so sticky, doesnt gum up bits as readily.

Some thoughts as i dont have my notes with me but worked up my feeds n speeds for aluminium doing this.

Check Winston Moy videos like this one:

Making an Aluminum Longboard on my Desktop CNC - #146 - YouTube

Use an upcut bit, as you need to clear the chips.

Shallow depth of cut and have a stepover (channel wider than bit diameter) can help with profile cutting thick material. Cutting slots with Al is not a joy, having a wider profile channel and finishing pass at full depth make things tidy.

1 Like

Do you know the specific alloy you’re using? I’ve had decent success cutting 6061 from a local metal supplier but on one occasion I had what I thought was 6061 but was much “gummier” and had results like you’re showing there. Try cutting a piece with a hacksaw and see if it creates chips/dust or just gums up the same as you experienced with the CNC. I don’t know what it was that I had, maybe 5052 or 3003 but it didn’t cut like the usual 6061 I get, no amount of tweeking the feed rate and DOC helped.

I also have an air blast nozzle to help cool and remove chips from the cut, it helped a lot with cut quality on aluminum.

1 Like

Rrpm as low as it will go, and spray WD40 on the top, and keep spraying it at the tool every few seconds while cutting to keep it wet.
As someone else mentioned, gluing the aluminum to a wood backer board will help too.

1 Like

I’ve also been cutting brass to make clock faces. The numbers have parts as narrow as 1/64" so I’ve tried single flute bits with tips of 0.005 and 0.01 " diameters.

The point about slow IPM is on target. Bit breakage improved at 5 IPM and depth of cut only 0.005".

JointCAM_Gerry recommended slow RPM, which is the advice I started with. But it depends on what you’re trying to do. With thick stock and ‘large’ bits, a slow speed reduces heat that actually melts your workpiece and adds to the mass that clogs the bit. However with thin stock and tiny bits, heat is less significant. In the second situation, the movement of the tip across a surface that hasn’t (yet) been cut results in breakage of the tip. I had to use the fastest RPM my spindle can provide. I’ve had better success with Amana bits than Onsrud. Further, the Amana folks engaged their engineers when I reported the third broken tip. It was those engineers who convinced me to use the fastest possible RPM. With a 0.005 tip, they wanted 50k, but my spindle tops out at 24k.

The alloy recommended for machining is 360, but few places offer that in thin plates. My substitute has been 260 Half Hard.

A big surprise for me was damage to my spindle caused by brass dust. I see no dust (using Oneida 3HP cyclone central shop vacuum). But the spindle picked up enough brass to ruin the bearings. The manufacturer (Mechatron, Pfungstadt Germany) suggested an air seal with positive pressure behind it. If you have an inexpensive spindle, metal dust may convert it from ‘inexpensive’ to ‘disposable’. If you want one to last, consider an air sealed device.


I was recently doing aluminum cutting. you probably already have an answer but my settings were
single flute 0.25" up cut
0.02 (max) doc
set at 1 on makita router (10k rpm)
(0.002 ipt, 600 sfm)

1 Like

Using a down cut is not a good idea IMO. The chips don’t evacuate. Check the bit to see if any aluminum has been welded onto the bit.

As others mentioned, the type of aluminum can play a big role in how it cuts. On the mill, I run bits slowly and lubricate with kerosene when cutting aluminum. Wonder if an IPA mist would be feasable without ruining the spoilboard?