Method for Finding Ideal Aluminum Parameters

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.

1 Like

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.

1 Like

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


I just went through and tightened all the bolts for the v-wheels and then checked their tightness to the rail. The bottom two X-axis bolts were not quite fully tight, but it didn’t seem to make a huge difference. However, I did notice that the lower right X-axis v-wheel appears to move the slightest amount relative to the plate when putting a lot of force on the spindle mount. I wonder if maybe the wheel ID doesn’t match the bearing (either a part quality issue or damage from running the machine like this).

Check the V wheels — remove each one and use the bolt for leverage to disassemble them — each is made up of:

  • Delrin wheel
  • a pair of 608 bearings
  • an eccentric spacer

Makes sure that the bearings rotate freely, and that the space is well-centered in the wheel and supported by the internal race — if you have a caliper, measure it and the race and let us know what you find out.


I realize it’s been a while since my last update, but after some more testing with the machine, I really think the issue was mostly due to my overestimation of what the stock machine could do and how hard I could push it.

Yesterday I installed my new HDZ and I’m extremely impressed with the results. I can now take much more aggressive cuts and still have better surface finish than before. The only weird thing I did notice while disassembling the machine is that it looks like my belt guide bearing flanges (on the original carriage) were rubbing on the X axis bar. I’m not sure how this can happen exept if the tolerances on the machining for the XZ carriage were off, but there’s quite a bit more clearance now with the HDZ and the machine is much stiffer.

I’ve also since received and installed steel reinforced belts and they also made the machine seem to behave better. I can tell the machine changes direction much more smoothly. Overall, quite happy with the results. I really wish there was an option to buy the machine as new with HDZ, because from my experience it seems like a requirement to do any serious Aluminum machining (one of my primary reasons for picking the Shapeoko over its competitors).

To address some of the questions above, I did look into the following items and found no issues:

  • Tool wear - took photos with a microscope and the tool was not damaged (may be getting dull by now though).
  • V-Wheel fitment - everything seemed fine here. When I removed the old v-wheels from the stock carriage there was no wobble between wheel and bearing. The only play in the system was between the threads and the inner race of the bearing. One thing I think could improve the system is using tight tolerance shoulder bolts here instead of fully threaded fasteners, but I realize that would probably cost 10-50x more than the current hardware.

I’ve finally had a chance to start a real project in aluminum so i thought I’d document my findings here for others to see. Only changes from a stock Shapeoko 3 XL here are steel reinforced belts & HDZ.

Here’s what the first part looks like. It’s part of a seat bracket for the racing seat going into my '89 Turbo E30 track car:

2D Pocket:

  • New Amana 51459-Z (1/4" single flute ZRN)
  • 20krpm, 1000 mm/min, DOC = 0.7 mm, WOC = 3 mm
  • Going to push harder on the next one, this cut very easily

2D Bore:

  • New Amana 51459-Z (1/4" single flute ZRN)
  • 20krpm, 800mm/min, Helix Angle 1.5°
  • These holes are only 8mm so not really the ideal end mill for this operation

2D Contour:

  • New Amana 51459-Z (1/4" single flute ZRN)
  • 20krpm, 1200 mm/min, DOC = 0.7 mm, 2 finishing passes (0.5mm) to prevent wall rubbing


  • Online Carbide 1/4" 3 Flute ZRN
  • 10krpm, 1500mm/min, DOC = 0.5 (rough) 0.2 (finish)
  • Single direction pass gave much better surface finish (still haven’t 100% trammed my spindle)


  • #202 1/4" 3 flute Ball End
  • Combination of hacked together 2d contours and scallop operations, didn’t work very well, but in lieu of having my chamfer cutters (in the mail from China), it’s acceptable. Lots of chatter and I don’t really recommend this.

I attempted a finishing pass in the pockets with 0.3mm DOC/WOC full depth w/ the 3 flute ZRN and it did not go well. Lots of chatter and I ended up gouging the floor of the pocket. In the future I will completely eliminate this tool path and just run to size w/ the single flute end mill, surface finish was acceptable.

Note on 3 flute cutters - I’ve found they are really only good for facing. In all other cases the single flute has given me a better surface finish and been way less scary to run.


Thank you for sharing, and that piece looks fantastic. I’m with you on the single flute bandwagon, they are basically unjammable (if that’s a word ?) workhorses, and I certainly appreciate the piece of mind that comes with using them.

Yep, I’m on the same page. I tried making a 3-flute endmill work for aluminum and found it only good for facing. However, I do find 2-flute endmills worthwhile occasionally as ball endmills come in 2-flutes and some other specialty ones are easier to find in 2-flutes than 1-flutes.

Edit: My knowledge is incorrect and I need to revisit these parameters again.

1 Like

Awesome looking part!

The single flutes require so much less tq and work so well with high rpm routers, plus wall finishes are usually better because runnout matters less.

Now if anyone made one with a slight corner radius…it would be indestructible! If you ever have a chance to try some Datron 4-1s I highly recommend it. The balance plus wiper really make a big difference. They also make a single flute ball mill :wink:

Was there a reason you didn’t try a 3d contour with just the touch area of the chamfer selected?

Again, awesome part and I hope you’ll be posting up more!


@The_real_janderson Hey Jon, thanks to some coaching from @Vince.Fab I got some pretty good results with 3flute coated bits from C3D using adaptive toolpaths, you might remember from last March. Need help testing cutters

1 Like

@Griff no problem with the 3 flute over here either…as long as you account for the extra chip evacuation needed and machine load/tq. Plus they are capable of awesome speeds!

1 Like