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!
{:0)
Brandon R. Parker
