1st try at aluminum

Well you know what they say “Go big or go home” so I thought give some aluminum (1/8in 5052) a try. I wanted 6061 but ordered the 5052 by mistake

All went well all though a bit slow (3-1/2hours) for a 5-1/2 x
2inch carve, I used their recommend settings of 5 in/min with a D.O.C.
at ,003, bit was an Generic 1/8" Single Flute Carbide Engraving bit (10 for $12 on amazon)

Text pocket is .03


Ah, the smell of WD-40! :wink:

1 Like

Once I started going faster - like 30 ipm, my cuts were much smoother. Now I go 35 ipm at 18k rpms. But I am using an 1/8" destiny viper bit. My depth of cut is also .003.

Thanks for the tip @Earwigger have to give that a try next time

1 Like

You can go a LOT faster.
I use 16k RPM, 2500mm/min, 1/4" or 1/8" 3 flute, 0.25mm DOC

EDIT: WD40 is not good for cutting, better use 3in1 oil.

Keep in mind, we’ve gone from single flute, to two flute, to three flute. Each jump requires a jump in speed.

Thanks guys I was hoping people would chime in with what and how they machine aluminum and you did

Got to love the the community here on inventables

After upgrading the spindle and stiffening the machine, I have run some long jobs on 6061 aluminum with:

  • 1/8" flat-end, two-flute, up-cut, carbide bit
  • DOC = .010"
  • stepover = .050"
  • IPM = 25
  • spindle speed = 18000rpm
  • and blowing a fine stream of air and sewing machine oil on the cut point

I really wanted to find a way to mill aluminum without coolant, but when cutting dry it always fails eventually with aluminum stuck to the bit.

Also, tried to make DOC=.020" work several times. Works for a while, but always fails eventually.

When I cut the Y axis braces for my 1000x1000 out of T6061, I used the 1/8" 2 flute upcut ball end mill from Inventables. 611 speed was ‘5’, DOC was 0.1 mm (.004"), and speed was 800 mm/min (31.5 IPM). I was able to cut this dry, with incredible results and no gumming.

@MattWheeler You’re going to slow. I can cut dry, without even air blower, uncoated endmill and no aluminium sticking to the endmill.

What width and depth of cut do you use?

These are my settings for AL:

RPM: 16.000 (dwp611 speed 1)
DOC: 0.25mm
FEED: 2500mm/min
PLUNGE/RAMP: 800mm/min

I use 3 flute 1/8 and 1/4 upcut no coating.

Yep, speed it key. I may try these settings as well. .009 @ 100 ipm seem deep for that speed. But… what the heck - I’ll give it a whorl with my 3 flute.

1 Like

Hi @CristianHinz - What step-over (width of cut) do you use with these settings?

Also, do you use “climb” or “conventional” direction tool paths?


I use 100% width usually with conventional

I’d love to see a video of you cutting aluminum with those settings @CristianHinz.

Whenever I use close to 100% width, the machine/bit deflects and a little sliver of material is left behind. If these slivers are left uncut for multiple passes, then they eventually cause the machine to loose steps because the residual sliver becomes too hard to cut on subsequent passes.

Ill try and make a video next time i cut some pieces.

Forgive me Matt - but what do you refer to when you say width of cut? When cut out a piece of aluminum, the bit goes into the aluminum at 100% width. Is that what you mean? I don’t know how one would go about doing less than 100% unless you were to create a pocket profile.

You can go less stepover with some of the operations like pocketing, adaptative clearing etc.

Btw, here are some pics of my settings on my last aluminium project: