Method for Finding Ideal Aluminum Parameters

I’ve been reading everything I can regarding machining aluminum on the Shapeoko and I’m still struggling to understand a few things. I realize questions about Aluminum are quite common, so if you’d rather I merge with another thread, just let me know.

In general, my question is what approach to take when developing cutting parameters for myself, less so on what parameters have worked for others. Right now I’m using some scrap aluminum from a project at work - very not ideal, I know - but I suspect it’s either 6061 or ATP5. I’m leaning toward ATP5 because it was quite brittle when I went to cut the supports to remove the first part.

What I’m really left wondering is where to go from here without damaging a ton of tools… Ideally I’d love to get to the point where I can make an entire part with a single end mill and not have to do tool changes, but with my current settings that doesn’t seem to be possible.

My settings for the two tools I’ve tried (approx, I was playing with feed & spindle speed to tune by ear):

  • 3-flute #201
    • Chip Load: ~0.025mm (20krpm, 1500mm/min feed)
    • Optimal Load: 20%
    • Ramp & Pluge: 400 mm/min
    • DOC: 1mm
  • Single Flute #278Z
    • Chip Load: ~0.116mm (14krpm, 1620mm/min feed)
    • Optimal Load: 20%
    • Ramp & Plunge: 400 mm/min
    • DOC: 2mm


  • 3-flute (#201) adaptive clearing
    • I think I’m not brave enough to move the cutter fast enough to generate a large enough chip to get good heat rejection
    • I ruined one end mill by welding chips to it (seems typical)
  • Single flute (#278Z) facing, boring, slotting
    • Anything besides an adaptive lead in doesn’t seem to work well. Both higher and lower ramp in/pluge settings created a ton of chatter and sounded terrible.
    • Very bad surface finish and chatter for these operations, swapping to a 3 flute and increasing RPM while using the same g-code was much more successful


  • 3-flute (#201) facing, boring, and slotting
    • Running slow plunge/ramp for boring seemed to work fine at 0.5mm/revolution
    • Facing worked great
    • Slotting was a bit sketchy, but overall surface finish was quite good (took 2 side by side passes, not just a plunge slot)
  • Single flute (#278Z) adaptive clearing

It looks like you have done your homework and are already getting pretty good results, so I’ll just add a few miscellaneous notes:

  • a jet of air directed at the cut will be a long way to clear chips and get uneventful cuts. You don’t seem to be using one ? (at least in that video).
  • bonus points for having a mister installed that will inject a small percentage of lubricant in the airflow
  • single flutes are excellent for cutting aluminium: better chip evacuation, less chip recutting.
  • you could cut with a deeper DOC since you are using adaptive clearing. I use helical ramping always.
  • I probably wouldn’t use a 20% optimal load myself, I’m more comfortable in the 10% zone for metals.
  • note that the actual chipload is lower than you mention, due to chip thinning, due to the 20% stepover.
  • which means the #201 chipload is probably a bit low (below 0.001") and hence the risk of melting, especially with a three-flute uncoated endmill. The actual #278Z chipload sounds right (after chip thinning)
  • I would have advised checking my intro to feeds and speeds, but it looks like you already know about all that?
  • slotting is always hard, and harder in metals: avoid whenever you can (i.e. use a smaller endmill and adaptive-clear a channel, to make the slot)
  • consider using a feeds and speed calculator to optimize your cut parameters ?
    @gmack produced the worksheet that rules them all, see :
    Speeds, Feeds, Power, and Force (SFPF) Calculator

Julien, much appreciated!

  • Right now I’m just vacuuming chips by hand. I am planning to use a coolant/lubricant mister eventually, but I would like to wait until I build an aluminum bed plate & I need to buy a compressor.
    • One thing I’ve struggled with is finding the required flow rate for most misting systems. I’ve seen numbers from 0.3 - 5 SCFM which is a huge range and if it’s really that high, would drive the need for a very expensive compressor (I suspect this is not the case).
  • I agree the single flute has had much better luck removing material, but I can’t seem to get it to work well when pluging into material. The features I’m struggling with are too small to use an adaptive cutting path with a 1/4" end mill, does this mean your recommendation is to use a smaller end mill and an adaptive path?
  • If the #201 chipload is low, and running minimum RPM still requires too high a cutting speed to reduce chatter does this mean I just need to use a different end mill?
    • I’m still not super clear on how feed rates work when plunging, I’d still like to find a way to make single flute work for all ops, but if it’s not a balanced enough cut to do it, I guess I may have to live with tool changes.
  • I will definitely check out your page to make sure I’m fully up to date, it’s been 15 years since school
  • Thanks for linking that calculator, I saw the output posted by VinceFab in another thread and I thought it was something proprietary he had developed, I’ll definitely start using that!

When I decided at the first of the year to save up for a S3 (will be getting it in January:grinning:) I found Winston’s videos and began following before he joined Carbide. I really liked his engineering point of view to find the best milling methods since I am woodworker and not an engineer. Anyhow I am glad to see that @wmoy has joined the Carbide team. If you have not seen his latest video on choosing the right material, in this case aluminium, its worth a view for all those who like milling aluminium! His point is that it’s not just about F&S. He has videos on other materials too and I bet he will become a great source.Thanks Winston! P.S. Loved your road trip series!


I’m sure Julien will respond shortly but I’ll jump in too with my thoughts below in bold.

1 Like

Personal experience: I have what appears to be the same one from Amazon, and can’t make the mister function with thinner wall tubing and lower pressures (50psi). In fairness, they do spec out “5-7KGF / CM2”, which is 71-100psi.

I had one just like that one that the valve eventually died. I switched to this one and have had no problems.

I ran both off my 8 gallon air compressor at 50psi with no issues running a 75/25 IPA/H2O mixture misting it onto my endmill.

Oops, looks like I forgot to answer. Basically, “what Jonathan said”.

  • compressor specs versus mister requirements : I am struggling myself to find the perfect setup. I have used a mister similar to the ones linked above, with my compressor, and it works fine but it’s LOUD, and since I do most of my cutting late at night, I need to find a better solution. I just purchased an air brush compressor, it’s very quiet but barely powerful enough, I still hope I’ll be able to find the right nozzle size that will make it usable for clearing chips.

  • smaller endmill to cut a wide channel using adaptive clearing, rather than a larger endmill and slotting: definitely.

  • yes, go to lower flute counts, it will help not only using a more reasonable feedrate, but getting much better chip evacuation.

  • plunging rate: there is (surprisingly) no definitive rule, my own recipe is documented here but even I violate that rule quite often. If you do helical ramping, the plunging rate matters less.


Thanks for the input everybody. I’ve done some more testing and I’ll share what I found.

In general I think I was being too aggressive in DOC which was causing excessive cutter deflection and chatter. In addition to sounding scary, it wasn’t doing me any favors for part accuracy or surface finish.

I still can’t successfully plunge the single flute tool, but maybe it’s been damaged by my previous attempts.

Working Adaptive Settings:
#278Z, 17krpm, feed 1050 mm/min, DOC 2.5mm, WOC 1.27mm, enter outside the part to prevent plugning

Working Boring Settings
#278Z, 17krpm, feed 1700 mm/min, 1.5°

Working Slotting Settings
#278Z, 12krpm, feed 500 mm/min, DOC 0.75mm, 2 radial passes, enter outside part - This is still very slow, but faster than an adaptive clear and doesn’t require as much real estate outside the part. I also found that preboring my entry hole works well since there’s no way in Fusion360 to force a helical entry with this tool path.

Working Facing Settings
1/4" 3 flute ZrN (OnlineCarbide), 24krpm, feed 850mm/min, DOC 1mm

Since this testing I have also tightened up the v-wheels and z belt so hopefully I’ll be able to push a bit faster without reintroducing chatter.

Here are the results. Walls were much cleaner, but clearly I need to improve my work-holding and tram my head.


Congrats on the shinies, and thank you for reporting your findings!
Here are a few thoughts

Indeed, usually one needs to choose between regular toolpaths at low DOC, high WOC, and moderate feedrate, and adaptive toolpaths at high DOC, low WOC and higher feedrate.

I guess you already know about that series of videos, the second one is of particular interest since it’s about using 278Z in aluminium. Winston’s recommended DOC for profile cut (slotting) is 0.38mm / 0.015", that’s 6% of the endmill diameter, which matches the guideline I usually follow (5 to 10% of diameter)

You can use a loupe to check the tip of your endmill, it may have been chipped (and then indeed, plunging won’t be fun). I avoid straight plunging as often as I can, helical or at least linear ramping helps a lot.

To reap the benefits of adaptive clearing, I guess you could go up to 6mm DOC, and I would personally reduce that stepover to somewhere below 1mm, and push the feedrate higher (HSM style)

What diameter were you boring ? It might be beneficial to use a smaller endmill and to a regular pocketing op, that way you’ll benefit from helical ramping, and then adaptive.

For comparison in the 278Z video, Winston uses 18K RPM and 914mm/min but at half the DOC (0.38mm). You end up having a similar chipload with your settings. Slotting will always be hard(er), and an air blast will help a lot.

1mm sounds a bit high to my taste for a facing operation ?
Also, 24k@850mm/min on a 3-flute is a 0.0005" chipload, near the lower limit, I would probably go 100% faster and 50% shallower


Julien, greatly appreciate the tips. I’ll give those a try this weekend!

I bored two holes, the larger was 12mm and the smaller was 8mm. I definitely found the 8mm hole was not ideal. In the future I will use a smaller end mill for holes this small.

1 Like

I’ve been continuing to tune my parameters and there are still issues with chatter on my machine. Still not 100% sure if they are settings related or set-up related. It seems like I get a ton of motion of the z-axis even though I though I had everything tightened up pretty well (as far as I was comfortable tightening it).

Is what I’m seeing normal? Is this the reason that people often upgrade their Z-axis to a ball screw? Or am I running into a different issue.

Here’s a video I took (Caution, Flashing Image! On account of the LED lights in my shop)

Maybe share details of the toolpath you were running at that time? Does it still happen if you reduce DOC ? Do you feel any play in the Z plate when you try to wiggle it manually in the front/back direction ?

1 Like

Julien, I was running an adaptive tool path at 0.05 mm/tooth (18400rpm, 950mm/min), DOC 2.5mm (all the stock that was available), WOC 0.8mm.

I can’t feel an wobble in any of the axes, and I’ve tightened all the v-wheels to the point where I can’t cause them to slip by hand. The Z-axis belt is as tight as I was comfortable getting it, it’s pretty tight. Maybe 50% more than either the X or Y axis.

I did have some issues with the router mount tram, so I fixed that today with some shims and it’s better but not perfect (perfect is somewhere between 2 and 3 sheets of thin aluminum foil).

Based on your experience, is this abnormal? Everyone says cutting aluminum sounds “bad” on the Shapeoko, but I’m not really sure what that means. At they very beginning and end of the video you can hear what it actually sounds like.

It does sound abnormal to me, like the endmill is bouncing on the material while cutting. Is this a fresh cutter?
note: to be honest I did very few cuts in aluminium with the stock Z axis before I upgraded to the HDZ though.

To confirm whether there is a mechanical issue I would maybe run a test cut in the exact same conditions as what Winston advocated in the aluminium series of videos (here)?

EDIT: I’m sure your wheels and belts are fine, I was thinking of that kind of wobble (just more subtle): (854.7 KB)
(it’s an example I downloaded from the Shapeoko’s FB group, rename file to “mp4” to view)

EDIT: to get a feel for what “normal” sounds like, check out the many videos in @Vince.Fab threads e.g. that one (835.4 KB)
(again rename to mp4)

or that old video of mine I grabbed while running an adaptive clearing toolpath. All of these are probably done with an HDZ though, but you get the idea.


curious if it’s the material.
most of those settings look fairly norm so it could be the mystery alloy itself.


I thought that was the case with the old material, so I ordered new stock from Howard Precision Metals confirmed 6061-T651 (“confirmed”, I didn’t actually request a material cert).

From looking at the video some more, it really looks like the Z-axis carriage is rotating about the X-axis.This correlates with the fact that the chatter is worst when the machine is cutting only in the Y direction. It seems like the cutting force from the single flute tool is causing this rotation but the system stiffness is just in the wrong place and it wants to resonate.

What I’m not sure about is if this lack of stiffness is coming from the v-wheel design (probably not, others don’t seem to have this issue) or flex of the Z-axis carriage itself. I just don’t want to spend $300 on an upgraded Z-axis if it’s not going to fix the issue.

I will run some more tests with the recommended settings, but from what I’ve seen from others, the machine should be capable of higher material removal rates. Maybe those people are all using upgraded machines. I just want to make sure I understand what’s going on so I don’t just end up throwing money at the problem.

In some (most?) of Winston’s videos on cutting aluminium on the Shapeoko, he is using a stock Z axis, so your approach of not rushing to buy an HDZ before you understand what’s going on sounds smart to me.

Your comment about it probably being the carriage rotating around the X axis still makes me think of a subtle assembly issue. Can you just confirm that when you grab the router mount and shake it up and down, you don’t feel any play/bending at all ?

Anyway, if you are going to replicate one of “Winston’s” cuts, same material and same cutter, we’ll know if it’s something about your machine.

For the sake of testing, and since this could be a resonance of some kind, you may also want to try

  • different RPMs ? (adjusting FR accordingly, obviously)
  • using feedrate override during a cut, see if the problem gets better or worst

As a triple-check, can you share your design file ?


I checked the stiffness of my machine:

Here’s an updated video of a 2d Contour OP using Winston’s settings:

Here’s a picture of the completed part:

If you’d like to take a look at my Fusion 360 model & setup:

I’m not sure if the end mill is damaged so I’m going to grab one of the Amana ones off Amazon.

that looks like a lot of flex in your stiffness vid…

attempted the same on a stock XXL and it didn’t seem to budge by comparison