Double checking my data before first attempt at aluminum

Hello all, I have done my best to research, but I just wanted to go over my workflow process before I start the cut. I believe it to be a relatively simple job.

Im cutting into 1/8" 6061 aluminum. The dashes in the center are an SVG file I have uploaded, and they only need to be etched onto the surface - anywhere between .2mm - 1mm. I have a 60 degree V coated carbide tip for this portion of the job. I am then going to change the bit to a 1/16" coated O flute spiral and use it to cut the etching out of the aluminum. The screenshot attached has the job being done in one pass with only with the V bit…I know to do them as two separate jobs.

I will be following Inventables recommendation for Carvey and aluminum as I found on their site " **Safe limits for Aluminum are as follows: 5”/min feed rate, 2.5”/min plunge rate, 0.003”/pass with minimum 0.0625” milling bit.*" although I have searched the forum and do see users using deeper passes than .0003" - any insight onto this?

Ive also seen that I need to use “Helical or torchoidal toolpaths like they have in Fusion 360”, but this is outside of my current level of understanding. I have Fusion 360, but I have barely used it. Sketchup is often fine enough for my modeling needs. Also, I pay for Easel Pro…is the pro version not capable of doing this?

Im a novice so I am just wanting to be sure that this is the right way to go about this. Im also not totally sure on if I should coat the aluminum in oil/alcohol/WD-40. If so, should I simply pause the job on the Carvey and lift the lid every few minutes to brush away chips and respray? Seems like a hassle, but willing to do it if it means it does the job right.

Thanks for any insight.

Hello @ZachSearcy and welcome!

For the project, you will want to take the cutout and move it to a separate workpiece. Currently, Easel uses the defined detail bit for any cutout within a project.

Just duplicate your workpiece, remove all of the items you intend to v-carve, and set up to use only the 1/16" bit for this new cutout.

On the original workpiece, remove the the cutout and set it up to only use the 60-deg v-bit.

I would do the v-carve operation first and then the cutout last.

The feeds/speeds from Inventables will be on the conservative side, but they are always a good starting point. IMO, the one that I would probably bump up would be the feed rate, but this is very dependent on machine rigidity, quality of bit, and grade of aluminum. For a 1/16" bit, you might be able to go two to three times (or faster) as much for the feedrate, but you should feel your machine out while it is actually performing the machining.

You will want to make sure you have several o-flutes at your disposal. While they are fantastic at milling aluminum, they can be extremely fragile. One mistake and that nice pointy tip/sharp edge will shatter to pieces on you. I mill a decent amount of 6061 and recently wasted two Amana 51377-Z (1/4" Spiral O Single Flute ZrN) bits at $50/bit on a simple bushing for an LS engine swap in a Subaru Forester. One ate it doing a rapid through a hold-down bolt head and the other called it quits when the part shifted during the final pass on the cutout. Both were my fault, but I guess my point is that mistakes will be makes and having extra bits on head is always a good idea when working with metal.

Since I have an X-Carve with particle board slats on top of an aluminum base, I do not use any type of cutting oil/coolant. In my opinion, oils & WD-40 tend to cling chips together close to the bit unless continuously flushed/removed which causes recutting of chips. I always cut 6061 dry on my X-Carve. If you get the settings correct, you can still get a really good finish.

Another word on 6061 stock… It will likely never be truly flat. This can cause issues when v-carving very small depths, since although the bit traverses machine space the same depth, it may not cutting into the material the same depth due to variations in thickness. This is very prevalent extruded plates. I would recommend running a flattening pass over the entirety of the part surface until you just slightly material across the entire surface. The outcome will obviously depend on how well your spindle is trammed.

On that bushing, I was using 3/4" x 3" 6061 flat extruded bar, and it was all over the place. On the first attempt, I had to remove 0.007" to flatten it over a 2.5" x 3" section. The second attempt had to go down to 0.01" just slightly down the bar for the same size rectangle.

Final bushing…

With bearing pressed in…

With respect to toolpaths, Easel does not always produce the best toolpaths, but 6061 is a “soft” metal and the toolpaths generated by Easel will work fine as long as you get the feeds/speeds dialed in correctly.

Sorry, I can’t provide you exact feeds/speeds to use, but these can vary a little from machine to machine. Since you have a Carvey, yours will definitely be slightly different than my X-Carve.

Also, I would suggest doing a small practice project or at least having plenty of 6061 stock available in case something goes awry.

Others will likely chime in with more pointers and their own experience as well…

Best of luck with your metal-milling adventure, and post some pictures of the progress!


Brandon R. Parker

Hey Brandon, thanks for you responding. It’s pretty amazing that youre able to mill something used in an engine. It still kinda blows my mind that this kind of stuff is accessible outside of a manufacturing plant.

I dont yet have a flattening bit for a flattening pass. Ill see if I can pick one up.

Noted on having several O flutes. My biggest concern is the cutout. Im pretty sure the V bit will do the etching quickly and without hassle over a couple passes. Im guessing the cutout is where I really need to hone in on my feed/speed the most. Feed and speed is probably where I lack the most knowledge as I am just finally getting my head wrapped around what bits are good for what.


On the Carvey, using a straight profile cut (not an ideal path through aluminum), you want to take very shallow passes. In general, a fast feedrate is ideal, but keep those passes shallow.
You can take deeper cuts with an adaptive toolpath.

So thats about twice the speed and exponentially deeper than .003". I appreciate theyre being conservative, but maybe I can increase those numbers a bit since it’s a softer aluminum.

Another thing you can do instead of doing a cutout is to take the shape for the cutout and do the following:

  1. Copy the original shape and change it to a pocket cutout with zero depth.
  2. Center this shape and send it behind the v-carve objects for z-order (or just bring them all to the top).
  3. Change the original to a pocket cut.
  4. Resize the original such that the width and height are:
    newHeight = (origHeight + (bitDiameter * 1.5))
    newWidth = (origWidth + (bitDiameter * 1.5))
  5. Send the original to the back of the z-order.
  6. Center the original on the other items.
  7. Change the cut depth to 0.020" shallower than the actual thickness of the 6061 stock.
  8. When the machine has completed carving, you can easily use a razor knife to trim the remaining aluminum at the bottom.

This will prevent the bit from having to carve deeply within a single bit width while preventing the part from coming out of the stock at the same time. This is exactly how I cut the bushing out on the last attempt.


Brandon R. Parker

As I said in that post… It’s all about the toolpaths. With Easel generated toolpaths, you’ll need to stay shallow.

Understood. Im in the process of googling, but are you familiar with any good articles or videos on how to generate these toolpaths in 360?

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.