Which of these bits should I use to mill aluminum?

I’m trying to mill some aluminum (to a depth of about 3mm) and after breaking half a dozen bits that were admittedly cheaper, I’m needing to find something that’s made for the job.

Right now I’m trying to decide between these two…

There’s obviously a big price difference between the two and I’m really weary of spending $25 on a single bit given how quickly I broke the last few.

Just curious if either of those should do the trick.

Here’s my project: http://easel.inventables.com/projects/qxoaq0Z6lZkl807itwJADg

You need to share your project. Use a solid carbide upcut bit, do not use the downcut. dust collection is a must, dust collection and air is even better you do not want any chips in your cut path. Setting 1 on the dewalt, shallow cut (.005) and fast feed (30-50ipm) The 51471 should be fine I also use drillman1 on ebay http://stores.ebay.com/CARBIDE-PLUS/DESTINY-TOOL-/_i.html?_fsub=2319753013&_sid=2877033&_trksid=p4634.c0.m322 The Destiny Viper bits are great.


+1 for @ChrisRice suggestion. I would use this bit for aluminum if you need an 1/8 inch one

1 Like

A few things…cheap bits that are fragile, potentially too deep of a cut…not sure what else?

Also, project shared (forgot to hit “save” last time).

1 Like

Just looked at your project are those the settings that you used?

They were the most recent I tried. I used half a dozen variations and they all broke the bits. The main thing I changed was I kept reducing the feed rate. 350 mm/min was the slowest I tried.

Take a close look at the end of the broken bit you will probably see it all galled up with melted aluminum. It is a huge problem to cut over chips in aluminum. Were you using dust extraction or air?

Albeit not an Xcarve, but my diy inc behaves similar to the Xcarve - with 0.1mm DoC (Depth of Cut) I usually go fast, around 1200-1600mm/min with a 3F uncut helix bit at 10K rpm (Makita)

I have had excellent result with these bits - http://www.ebay.com/itm/Lot-5Pcs-Solid-Carbide-Aluminum-End-Mill-3Flute-Cutting-Dia-3mm-Shank-Dia-6mm-/122670973669?hash=item1c8fc282e5

I concur with @RickPeterson . The Destiny Viper bits work very well with aluminum. .005 Depth with a 40% step over at 50ipm has served me well and they last and last and last. Check tramming. That is critical when milling aluminum.

Charley Thomas


If you are breaking viper bits then your settings are wrong. Viper bits are generally accepted as very suited for milling alu.

Breaking bits will most likely happen from bit getting “gummed” up.
=> bit rubbing more than cutting / rates too conservative.
Machine rigidity also play a factor here.

I’m no expert, but I’ve probably got about 40-50hrs cutting AL on my X-Carve for the High School First Robotics team I’m mentoring. I gave up on cheep bits a long time ago. I don’t really use my CNC enough to warrant penny pinching on the bits. A good bit will last me a long time so I don’t mind spending a little extra (even 10x).

I really like the single flute Amana Solid Carbide Aluminum Cutting Up bits (51417) for routing parts out.

I have found that I can run a 3/16" bit faster than the 1/8" bit. The 1/8" bit flexes too much and will chatter sooner. The 51417 bit has a 1/4" shaft which helps reduce flex. I tried a 1/4" cut, but found that I had to go slower due to system flex and not really having enough power to cut the AL faster. I added stiffeners to the X and Y axes, but still run the stock Z-axis. I also agree that you need to have a vacuum or compressed air to remove chips. As soon as you start getting any chatter, stop or you’ll be dealing with a gummed up bit. The one downside to the single flute is that it does not plunge cut well and will wobble as it goes in. So it does not make circular holes well.

For plunge cutting holes I use a two flute 1/8" Kodiak solid Carbide end mill:

The Kodiak looks and price are similar to the Destiny bit talked about above. I have not used the Destiny bit so I can’t compare them though. The Kodiak does a great job of plunge cutting holes, but it does not side cut as well as as the single flute Amana. So if it is a big job, I tend to use the Kodiak to plunge cut holes first, then cut out the actual part with the Amana.

1 Like

My vote would be the Kodiak

use this tool you will like it and lol

dont worry about the price they are all expensive I have spent over 1000.00 this month alone in tools for different jobs and I just place another order this morning for a single .125" compression spiral at 50.00 each

tooling is the number 1 expense when running these machines but with the jobs that come in your customers should be paying for these tools or at least part of them