Machining aluminum on XXL

I have machined wood successfully on my XXL, and I have machined aluminum successfully by hand. I now want to start machining aluminum on the XXL. In the past, I needed to lubricate the end mills frequently in order to prevent adhesion of aluminum onto the cutting surfaces. Real metal CNC machines often flood the parts with lubricant, but I want to avoid that if possible.

Can someone point me to a FAQ or white paper discussing how to set up the proper end mills (geometry, materials) and feeds and speeds to allow me to mill aluminum on the XXL without the need for lubrication?



The last time I cut aluminum I just used the feeds and speeds in Carbide Create and cut dry w/ dust collection (the Sweepy I used is a bit hazy now from the scratches).

Things which will help:

  • use an endmill w/ a suitable coating (the coated ones in our shop are all suited to alu.)
  • clear the chips
  • set initial Z-axis height accurately
  • rigid workholding

There’s a bit more in the various videos at:


I have great success machining aluminum without any lube 90+% of the time as long as the cutters are ZrN Coated.

For the few times that lube is needed, I use my WD40 Drip can system.
Link: My World Famous Shapeoko WD40 Drip Can - YouTube

Note: While the XXL is an oversize S3, please remember that the machine has the highest rigidity at the 4 corners…as opposed to the middle of the machine (where dampness is the lowest)


Rich, I’m most curious to know the circumstances that require lube from your machinist/engineer perspective.


Deep narrow slots…where diameter to depth exceeds 3 (e.g. 1/4 wide slot that is deeper than 3/4" (Yes blowing the chips would help…but also messy).


90% of what I cut on my machine is 6061. Here are the general rules I use:

  • Single flutes work best, 2 flutes can work if you are careful with chip clearing
  • Avoid deep slotting if you can
  • ZrN coated tools work really well but are not required. Most of my tools are uncoated.
  • Stick to low DOC and high stepover strategies. For example, if I was going for fastest material removal on my S3 prior to my upgrades I would use an adaptive toolpath at 0.03" DOC, 75% radial load, 24K RPM and 72 IPM with an 8mm tool. I would go down to about 60 IPM if I was using a 1/4" tool.
  • Use helical or ramping entry strategies. Plunging into aluminum is not fun. If you don’t have a way to program this kind of entry, use very small stepdowns.
  • Try to only cut 6061 or similar grade aluminum. Other types tend to get really gummy.
  • Make sure your chip clearing is adequate. I use a dust collector. Air blast is also good.
  • Make sure your chipload is 0.001" or higher on 1/8" tools or larger.

I’ve cut a dozen or so aluminum swords this week on my XxL and it did great. I used the speeds and feeds on the C3D doc and found it did well with an occasional squirt of WD40. Building an enclosure for it at the same time so my shop sounded like a jet engine…

1 Like

Will any old 1 flute work, or should I purchase end mills especially designed for aluminum?

You can get away with non-specific cutters but a single flute designed for plastics is likely to fail or blunt pretty quickly. You can use two or more flutes but these risk gumming up in pockets unless you have air blast, lubricant or other assistance. Single flutes and coatings all help to minimise this.

A metals (preferably Aluminium) specific cutter will work best and last longest.

Coatings can help, but avoid anything with Al in the coating, e.g. TiAlN. I like the DLC coated cutters as I’ve had some success with those.

Lubricants help, oil based or Isopropanol, WD40 etc.

You should be able to find a cutting tools supplier with decent cutters at reasonable prices near you. Here’s one I use as an example

I’m really enjoying the 1/4" and 1/8" single flute aluminum end mills from 2L. They seem to be lasting well and the 1/4" works great for adaptive clearing big areas.

I have always used cheap-ass crap end mills from Amazon (uxcell). I have used 0.8mm and routinely use the 1.5mm and 2mm. These are all 2 flutes but I mostly use them for boring holes and that doesn’t generate a huge amount of chips.

The videos referenced above discuss Pocketing, Contour, and Adaptive tool paths. I will be using MeshCAM, not Carbide Create. Which kind of too path does MeshCAM use?

I have some experience with metal machining- as the routers often exceed the RPM’s for metal and thus generate significant heat from friction , causing aluminum to melt , gall with distortion of the metal. Flood coolant is best, but the most challenging to use on your carver unless your setup enables the reticulation of the coolant and filters all the time. Second best and less mess is mist coolant that is air pressure causing a velocity of moist lubricant that is misted on the surface of the aluminum. Note that You Tube offers some insight, but you’ll need some research on what type of lubricant - Understand that the mist also poses other issues such as air-born particles ou don’t want to inhale. CNC Router Aluminium with mist coolant. - YouTube Tom

Having coolant is a nice thing that helps with finishes but it is not required for cutting aluminum on these machines unless you a really pushing the machine hard. I have been cutting aluminum dry for several years on my S3 at 30000 RPM on the router and now 24000 RPM with my spindle. The key is using single flute cutters and taking a healthy chipload.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.