so I bought without asking first my first bit to cut aluminum. Now that being said I bought a 1/4" x 2 1/2" Solid Carbide Ball Nose 3 Flute End Mill .
Now My question is What would you prefer I do as far as Feed, Plunge and Depth. I wish I were smarter with this kinda stuff and hate to ask, but I need help-thanks
There are a number of aluminum cutting threads on the Carbide3D forum. Members have posted feed and speed info that you could use as a starting point.
1 Like
I’d try to get a starting point from an X-carve user. Different animals. I don’t think an X-carve can be pushed the same.
I’ll be honest with you, a three flute end mill is probably not ideal for these machines as they have an increased material removal rate which will require even higher feed rates these machines generally cannot do. You’ll have to compensate with shallower passes.
This also REALLY depends on the toolpath. What are you using to generate toolpaths?
Just some tips on cutting aluminum… I’ve never done it cnc on the x-carve, but I have 2 Bridgeport milling machines and do a lot of machining there… “Ideally” when cutting aluminum, you’ll want to use some kind of lubricant… a lot of shops use Kerosene… that being said, you might wish to find some way of protecting your waste board… additionally a High Helix end mill is preferable in aluminum. It gets less clogged with material… if you’ve ever tried drilling a hole through thick aluminum, you’ll know that the tip of the drill almost always gets clogged up with material unless you are very careful. 
I’m not milling aluminum yet but following other threads on the subject, people use a compressed air nozzle to cool the bit and clear chips with great success. This has the advantage of not ruining the MDF. Some who have an aluminum wasteboard use a WD40 drip in some circumstances, I think it is probably safer than kerosene.
As I mentioned, there are several very good threads on the subject on the Carbide message board and while the information needs to be adapted (dialed down F&S in particular) to the capabilities of the X-Carve, they provide great information on the type of bits, feed and speed, hold down, bit clearing, cooling etc. All these should be very useful to aspiring aluminum milling enthusiasts.
If you select Aluminium, Easel has some default settings. Try those and work from there.
I wouldn’t recommend Easel for aluminum. I would also throw Vcarve Pro and Aspire into that group. Those are primarily wood carving applications. Milling is greatly affected by toolpath design, Easel/Vcarve Pro/Aspire just don’t have the advanced toolpaths that allow the X-carve to hit it’s full potential. You certainly can use them, but you’ll be risking your tools and your time. For a quick one-off job, it’s probably not a bad option. I would recommend Fusion 360 if you intend on doing aluminum milling with any frequency. It’s free as well.
2 Likes
I use Vcarve routinely to cut 1/4" 6061 aluminum plate. Works fine for me.
For basic stuff like slots and profile cuts, Vcarve Pro has enough control to make it functional, sure; however, with a proper adaptive clearing pass in a milling suite you can decrease toolpath times by magnitudes over wood carving software, and really get the most out of your machine. Vcarve Pro and Aspire simply are not made for milling, they lack some of the most basic milling toolpath operations.
Now, clearly the OP is just cutting his teeth here, and depending on what his ultimate goals are Easel may serve him just fine. But if he wants to progress into milling, buying an expensive software suite like Vcarve Pro over a free software like Fusion 360 would be questionable.
I love Aspire for wood work, and I recommend it if you’re going to be making vcarve signs, or using 3d clipart in wood, there’s nothing faster.
1 Like
What settings do you use for your teeth? Will masking tape and super glue work here?
1 Like
lol
1 Like
I have used my x carve to cut aluminum many times .you have to understand that the x carve is not a heavy duty milling machine. You must make thin cuts and slow your feed rate. This will help lessen deflection and chattering. Remember you are working with a cnc machine and it will make multiple passes. I have made sinker molds with good success. I used a 1/4 inch 4 flute carbide end mill to rough out and finished the 3 D cutting with a 1/8 inch carbide 4 flute ball end end mill. I did not have to use any coolant. It takes time but the final parts came out good. Hope this helps.
I got the X-Carve as an affordable solution to building parts out of Lexan, HDPE and aluminum for a high school robotics team. The aluminum has been the last challenge to overcome, but here are my thoughts and findings (some I figured out on my own and others were information from my peers in the robotics community):
- Easel is OK for the basic work that I do. We may design a part in Autodesk Inventor and then import it, but Easel is reasonable.
- I installed but have not used air clearing jets like others have talked about, but the cuts we use are about 30 minutes or less (not hours). We notice that the shank inside the router gets warm with each cut, but is certainly not hot and the tip is not even warm at the end of the cut.
- We do not use any lubrication for these cuts. I tried WD-40, but found no difference than a dry cut
- The wasteboard has to be level in relation to the X- and Y-axes.- if not, your first pass will likely lead to deflection wherever the board is highest unless that is also where you set your Z-axis depth
- The material has to be completely anchored. Any looseness can lead to chatter and broken bits.
- We change the settings in Easel to Feed 40-45 in/min, plunge 1 in/min, depth 0.04 in/pass
- We use an Onsrud single-flute HSS bit. We have been successful with these settings with the 1/4" and 1/8" bits
- We have used these settings and bits on 1/16" and 1/8" 6061 aluminum with good success
You may have completely different needs than we do, but this could be a starting point. I have attached a picture of our latest robot. The yellow words and stars in the picture were cut out of 2x1 box aluminum and have a LED strip light inside to illuminate. There are several other things on the robot that we cut such as bearing holes, etc. that are not visible in this picture
Forgot to add - the Dewalt 611 is set on speed “1”
Hi , I’ve been cutting a lot of 5052 alloy on my machine , lots of trials and failures , best results are with a single flute cutter , no coolent , no cutting aids … think big chips and shallow cuts
Unfortunately I don’t have my f&s numbers in hand but one of the first things I made with my xcarve last year was a corner finder I milled out of a 1.5"x1.5"x1" block of Aluminum. I used a 1/4" 2 flute mill to rough it into shape and a 1/8" single flute to clean it up, no lube. I guess the point I’m trying to make is that it is possible to mill Aluminum well on the xcarve.
One thing I found helpful in understanding what to expect was looking at videos of machines milling Aluminum. Two limits on the xcarve are machine rigidity and power. The xcarve has plenty of both for wood but with aluminum you can’t run the same high feed rates unless you do proportionately shallower passes. In those videos I mentioned I noticed slower spindle speeds, slower feedrates and the depth of cut a function of machine power. So I picked a feed and spindle speeds then varied the depth of cut to get an adequate material removal rate.
The increased power required will also demand sturdier clamping of the stock. I remember struggling with this more than with the feeds and speeds since any give in the setup immediately causes chatter and I kept thinking it was my f&s settings…
Good luck!