Machining Aluminum

Hello Everybody,

I have a few questions about milling aluminum. I have done the basic math regarding feeds and speeds… Theoretically, I’m all good but I have never cut aluminum before and I don’t really know the limitations of the machine (set it up a few weeks ago).

I have cut various woods using the standard calculations and have gotten pretty decent results. Can I do the same with aluminum?

  • Feed Rate (IPM) = RPM * # of cutting edges * chip load
  • Plunge rate = 50% of feed rate
  • DOC = 1x Diameter

Endmill Info

  • LMT Onsrud #63-610
  • ⅛’’ Diameter
  • ½’’ LOC
  • 1 Flute, upcut
  • Recommended chip load: 0.002-0.004’’

Machine Settings

  • RPM (Makita): 10,000 RPM (1)
  • Feed: 30 IPM
  • Plunge: 15 IPM
  • DOC: 0.125’’
  • Resulting chip load: 0.002’’

I am mainly confused about my DOC, the manufacturer recommends 1x diameter, but that seems a bit aggressive.

Referencing this datasheet for my cutter, do the above parameters seem reasonable? Is there anything I should change? I am currently using carbide create.

Thanks for your help!

1 Like

That DOC does seem a bit much for aluminum, although I haven’t had any experience with using 1 flute end mills. When I do aluminum, I usually do .060 DOC with feedrate of 30ipm (4-flute end mill), but I usually back down the feedrate by 50% until I get a feel of how it’s going to do. It also depends largely on my setup, and if I’m running cutting oil or not. Then bump up the feedrate as I see fit. But I’m usually doing paid jobs where the overall tolerance must be +/- .005, so my main priority is making sure I get a good quality cut. I’m not running production, so I’m not in a hurry. Just enjoying the project.

I found this video to be very informative.
Shapeoko Feeds & Speeds and Machining Tips! - YouTube
1x dia. DOC is only if your machine is built like a rock. Actually i think the 1F is strong enough, but if it’s a Makita router, that may put too much flex/vibration in the tool. Not saying it can’t be done but tool life may suffer severely. Mainly from not having a high enough feedrate to stop the cutter rubbing.


Hi Bill,

Thanks so much for your advice! I am part of an FRC robotics team and also need parts to be within 0.005in and churned out pretty quickly, obviously not prioritizing quality over time…
I think I will start out with a DOC similar to what you use and work my way up. Do you get a lot of chip welding with the 4 flutes, even with cutting oil?

Thanks for the video Chris!

I think I will start off with a low RPM/feed and then work my way up. What DOC do you normally use for your 1/8in bits?

1X DOC isn’t an issue as long as your radial stepover and chip load are adjusted for. Just keep in mind that although the 1F machines are very rigid for what they are, they are still less rigid and contain much less mass than a proper VMC. Use an adaptive strategy with stock to leave and then clean it up with contour and/or horizontal tool paths.

In the first pic is a .25" 2 flute end mill on my 1F machinist model. Second pic is the chips from the cut. Hope this helps.


You’re very welcome, and best of luck with the project. Yes, chip welding can be an issue (generally only without oil). Sometimes I attempt cutting without oil (for example, when my part is stuck to the work surface with 2-way tape). I just had a job this morning where this was the case, and I started getting chip weld. I was right there babysitting it, so I swapped in a new end mill and finished up the job. I will salvage the end mill later. I backed my DOC down to .030 with a feedrate of 20 ipm, but backed that down to 20% to start. With small parts stuck down with tape, you really have to be careful of pushing the limits of adhesion of the tape, lest the part should shift. I’d rather finish the part at a snail’s pace & not have to start over because of part shift.

Thanks for the reply. As of right now, I am only doing super simple 2D work (outer/inner contours), mainly gussets and gearbox plates for our FRC robot (student competition).

You mentioned the use of an adaptive strategy, what CAM software are you using? Our team is currently using Carbide Create (for CAM). Fusion360 is not an option, as our team (along with pretty much the rest of the FRC community), uses SolidWorks. Is CC sufficient for 2D aluminum? There is Solidworks CAM and I believe we get a MasterCAM license but I’m looking for something simple and easy to use, especially for new students.

Looks good, is that a handle for a knife?

No problem, always glad to help. I use Fusion 360 for both CAD and CAM. Yeah if you are looking to keep tight tolerances and cut quality I’d look into Fusion or make the jump to solidworks and Master Cam. Both Fusion and Solidworks are substantially more powerful than Carbide create. Not that it won’t do the job or to bash it or anything as it is good for the market it was designed for and is a great primer for new students. There is a point though where moving into a more powerful software suite will take your design and programming to the next level. And incorporating the engineering aspects of the software packages like creating movable joints, stress/load analysis and mass allocation could be a big advantage for your team.

Hope this helps👍

Thanks! No, this is some sort of part I made for an Xometry customer, not entirely sure what it is. But this is very typical of the parts I take on for them, mostly just 2D profile parts in thin aluminum or other plastic-type materials.

1 Like

If you are machining Aluminum (Aluminium) using Carbide Create then I would look up Winston Moy on The following Youtube Channel as he has done a few decent videos on the subject. Albeit he is using the Shapeoko/Nomad machines which they sell.


Thanks Dave, I’ll check it out!

Sorry, I should have been more clear, we do use Solidworks for design/modelling but Carbide Create for CAM (not design). Regardless, you have been super helpful, I really appreciate your (and everybody elses’) comments!

1 Like

Like virtually all other CNC routers, the ultimate weak point (particularly when machining metals) is the Z axis. The Z axis sub-assembly is 2x removed from the solid base of the machine, meaning that any play in the X, Y, and Z axis is ultimately absorbed and manifests itself @ the tip of the cutting tool. Now there’s not much play or slop in the X & Y axis, but the Z is substantailly smaller and there is only 1.5" of tool holder hanging onto the router. In addition to this, take into consideration that the tip of the average tool is going to be about 4.5" - 5" below the centerline of the 1.5" router holder. All that adds up to a good bit of leverage working against you when machining metal. Chip-load calculations are great and I applaud ppl that put that much thought into the process. I personally don’t, mostly because I’m an old-school manual machinist and everything was done primarily by seat-of-the-pants feel & gut instinct. But back to chip load calculations & derived feeds & speeds: these calculations are based on ideal machine setup and rigidity. The calculated feedrate may work well for someone running a Onefinity or better, but Imagine our stock X-Carve brethren applying the same prescribed feedrates.

Apologies for the endless rambling, I hope to instill some additional food for thought. :slight_smile:


No need to be sorry, your advice has been super helpful! I’ll be completely honest; I only learned about feeds and speeds when I got into CNC last summer. I’m 17 years old and I have been using a manual mill since 13. A lot of our machining on our team is done by ear and seeing what our (rickety) machines in the shop can handle :joy:. That being said, our first cut with alu went really well. Knowing those cutter recommendations are for industrial machines, we backed it off quite a bit and got a flawless cut!


Kudos for that! That’s actually some of the best experience you can get. Understanding the limitations & how wear can affect machine accuracy is key to becoming a well-rounded machinist. You will notice most well-used & ragged out mills will display more wear in the center of travel where most of the work has been done for years. You will learn (or have probably already learned) that the table brake lever is your friend when working in the ‘slop zone’.


Great thread! Would love to know what specs you used for that flawless cut! I planning on machining aluminum for the first time also and this thread has been super helpful!!!

Hey Luis,

I am putting together a post with everything we did. I am just waiting to go back to school so I get some better pictures. In the meantime here is what we ran:

Machine: Stock Woodworker, Makita Spindle + cutting oil
Endmill: LMT-Onsrud 63-600 1/8", Single flute
Spindle: 10,000RPM (#1 on the Makita)
    DOC: 0.020"
   Feed: 20ipm
 Plunge: 10ipm
  Stock: 0.10" 6061 Aluminum 

We only did a contour/2D cut, so I haven’t yet played around with the stepover. In our second cut we bumped up the DOC to 0.030" and it seemed to handle. We are aiming for at least 0.050", but like many people said, start low and work your way up!

17mm wrench for scale. Ignore the little dent near the bottom, that was me trying to remove the tabs :pensive: We sanded the part with some 120, filed the edges and voila!

The worst part of the cut was the fact that we used Carbide Create. It doesn’t ramp while plunging, putting a significant amount of stress on the cutter and sounds horrible.

Good luck with your cut, and let us know how it goes!


Awesome! Thanks for the info!!! I will update when I get a chance to run my first test. Thanks!!!