X-carve Mic-6 Aluminum Project

Alright, so I need to make a flat aluminum table for a project with a bunch of pockets in it, and have beefed my x-carve up for this very purpose (steel rigidity mod, 1.25hp spindle, 175 oz. Nema 23’s )

I only have the one plate, and am ok with doing a couple test cuts on the underside to make sure I have my settings right but for the most part I only have one chance to mill it properly. I chose Mic-6 toolplate since it has a very uniform flatness, and it was the right size I needed and was cheap too. I stupidly decided to do a test cut with a general purpose single flute carbide bit that I normally use for plastic and it instantly clogged the flute with aluminum and just rubbed and was super gummy and chattered like crazy even when being extremely conservative. When I attempted to use the speeds and feeds others have used in aluminum it just didn’t even mill, it was just rubbing, so at this point I have ruled out everything but the bit.

I will purchase a proper aluminum cutting bit and then try again, but because i only have one real try, I would appreciate if anyone had any speeds and feeds recommendations or just tips to throw my way, as I couldn’t find any info relating to mic-6 toolplate on here.

Here is the Easel link to what I am trying to do, nothing crazy, just some pocketing and some circles.

And for reference, this is my machine, and its rpm range is 10,000 to 30,000

1 Like

Id limit the depth per pass to ~.01" and keep the feed rate relatively high, like 60ipm ideally at ~18-20k RPM. 95% of the time when chips weld to the end mill its because of poor chip clearing. Re-cutting chips will cause a massive increase in heat and thats when they weld on and can lock up your spindle. While you have a dust shoe (which is better than nothing) to cut aluminum ‘properly’ you need a cooling system, air blast at a minimum. I have 2 of these outputting ~25-30psi each.


Since this is a 1-time cut, you can probably get away with manually clearing the chips with canned air or a compressor hose. I’d keep a constant stream of air blasting on the bit, making sure that wherever it is moving to has no chips in it’s path so it gets a clean cut.

Also, what thickness aluminum, and what size bit were you going to cut with?

Without a doubt I would use a Destiny Tool Viper end mill on this project. You can also look into forced air clearance system like i use which is you have access to a 3d printer, will costs you about $20 total and will keep the end mill free of chips without issue or needing to buy a compressor. The tool plate aluminum I mill in is 95% match to MIC-6. Just mine is more gearing for being anodized than MIC 6 is. So feeds and speeds will be the same overall. You need to figure out if you want to use a roughing pass (and good roughing end mill) or if you re going to try and do everything with a few DOC passes and on final finishing pass with the same end mill. I do not use Easel so I am not able to see the project nor the size end mill/s it needs.

But above all else you need to keep the chips clear of the end mill and keep your feeds and speeds in a good range for your end mill. I have tried MANY brands and styles of end mills for working in tool plate AL and time and time again the Viper gives the best finish hands done and the least amount of chatter or issues. They can be found for $11-$18 on ebay for 1/8" sizes… 1/4" is only about $22ish and well worth it if you need large areas cleared.

I cut my projects slower than most folks like, but I demand a perfect finish and very tight tolerances (for the XC) so I do not make fast rough cuts on my projects. My clients love the finish and I am slammed with orders so I guess something is being done right. I run the Viper around 15000RPM with .35mm DOC and 575MM/M feedrate. Those might not work for everyone, but for my with my chip clearance system, they work great and produce a perfect mirror edge on my parts every time.

Try the trial of G wizard and play with feed rates and DOC and such and it will give you an idea of where to go… Just keep in mind that overall it is geared towards BIG mills, the XC is a toy for it. So make sure you fill in as much as you can about your mill and take the feeds with a tiny bit of salt.

Keep us posted how the project goes or touch base is you need more help.

1 Like

this is off topic but I love the dust shields on your machine.

What are they made from, do you have any details on the cut and construction?

They are actually pvc sheet that I just cut and bent with scissors, I also used this same sheet to form the shim for my makita router. I don’t know where to pick it up, I got it for free out of a plastic suppliers junk bin :stuck_out_tongue:

Can you send me a link where you find the destiny viper bits? I only found a few on ebay for 24-30$ I only need the1/8" bit since I don’t have to clear any large areas. Thanks so much for the help by the way :smile:

would removing the dust shoe and vacuuming out the chips directly from the cut path be okay, or is an air blast really what I need, I don’t have an air compressor, and not enough canned air for the whole job. Is there any cutting lubricant that would work well? Ive seen people use ethanol as a coolant, and I have plenty of that.

Removing the shoe and using the vacuum by hand will probably work well enough. Lubricant is great, but in terms of preventing welding, its 2nd in line to chip clearing. Since you probably don’t want to invest in a compressor and air nozzle and all that jazz, I’d just use the vacuum to clean up as much of the chips as you can, and if you have a free hand get some lubricant in there. It’s gonna get really messy really fast if you use lube, and it will get harder to vacuum the chips out (since they have a tendency to stick to everything once wet). Its also worth noting if you are using lube and no dust shoe you should probably get a respirator of some kind just so you don’t breathe in ethanol covered aluminum dust.

If you are cutting and spray the lube on and it smokes up instantly, you need to stop the job and lower the depth per cut, you are creating too much heat and its gonna weld soon (or you can seriously dowse it in coolant to bring the temp down fast, but whenever I do this I usually have to stop it anyways cause my garage will fill with smoke).

Its also worth noting that you can aid chip clearing by letting the tool stick out a bit more. This just gives the chips more room to escape instead of hitting hte spindle and bouncing back down onto your part. I had my current setup (with air blast and coolant and all) and because I was using a “stub” end mill with none of the shaft sticking out (total stick out was like .4") I would weld chips no matter what I did. Aim for ~.75" stick out unless you are cutting like .5" thick aluminum, in which case I’d increase it a bit more.

This is all assuming a 1/8" bit (stock xcarve will not like a 1/4" bit in aluminum).

1 Like

I was reading an older thread where you discussed AlTiN coated bits and how they work well with aluminum because the coating keeps them somewhat lubricated. Do you still use these bits?
[1/8", 2 Flute Bit] http://toolinghouse.com/ESC1007U.aspx

1 Like

No! Don’t use them! AlTiN coatings actually wear out extremely quickly in aluminum. I’ve since switched to using either the Destiny Viper bits @Travelphotog discovered or anything ZrN coated. As of late I’ve been using 3 flute variable helix ZrN coated endmills in 1/8", 3/16" and 1/4". Typically I take a roughing cut (full cut width) and finishing pass (.005"). The results have been excellent.

Check out these (with ZrN coating, no chip breaker):


Expensive? Yes. But they will last 2-3x longer than uncoated/altin/tialn (so long as you don’t clog them up first).

Here’s the Destiny Viper bit, too:

I’ve researched some other coatings too, but they are pretty rare. PVD Diamond is top of the line. There’s also TiB2 coatings, but they are pretty rare (and I haven’t gotten my paws on one, either).

Also, I recommend getting an EM with a very small corner radius (like .005" or less). This can reduce stresses and reduce chatter.


Thank you for the great suggestions!

What exactly is the chip breaker, and why should I not select it? Also, should I purchase a square end EM or ball end?

You can try the chip breaker, I haven’t used it. In theory it should help with chip clearing, but at the cost of surface finish. Square end mills are for 2.5D work and ball end mills for full 3D work.

You’ve been a huge help, thanks so much. One last question, what chip load size should I try to achieve? I’m assuming it varies from bit to bit

Eric, Can you post a picture of your setup and how you mounted the mist system you pointed out.

I don’t understand why a blast of air clearing the bits would be that much better than a dust shoe with a vacuum sucking up all of the bits

It’s easier to blow chips away than to vacuum them. I’m not sure what the reason is (mass, adhesion, etc.), but metal chips do not vacuum easily from a dustshoe distance.

It comes down to a few things which make air blast/blowing better than vacuum sucking the chips. One reason is because the chips are heavier than wood chips and tend to resist being sucked up far more than lighter wood chips do. in a deep profile type cut or a slot cut, the chips tend to stay in the bottom of the cut instead of being sucked out and removed. Over all a dust shoe is meant to suck up wood chips or as it says, dust and not heavier metal cuttings. By having a forceful stream of air, you can direct the air stream to the base of the end mill to aid in lifting the chips out of a deeper cut. But having two or more streams from different directions you can very effectively remove large amount of chip load from rather deep cuts with ease. My personal preference is for forced air clearance with a small cage fan setup which is produces far less noise than a vacuum running for hours during a large aluminum milling project and is also is far cheaper then a compressor. The one down side to forced air clearance vs pressurized air clearance is that forced air is not able to introduce misting coolants unlike pressurized air clearance which can also convey coolant in the same air stream effectively.

Here is where i buy most of my Destiny end mills from. http://www.ebay.com/itm/1-8-carbide-endmill-for-aluminum-milling-coated-3-flute-Destiny-Tool-V30805S-/381528186619?hash=item58d4da1efb:m:mB6EV486fHjorKMn2EtgwMw He is a great seller and keeps them in stock 90% of the time. This will allow you to mill up to 1/4" or so stock with ease, not DOC but total depth of stock. Just always check you LOC to make sure it is greater than your desired deepest cut in a profile run.

Let me know if you need anything else and looking forward to seeing how your project turns out.

1 Like

I think it would be best for me to go with a dust shoe paired with a dust collector. I’m not only going to cut aluminum, I will also cut other materials such as carbon fiber, and you can’t have airborne carbon dust. Having a dust shoe will also eliminate the need for shields to protect the rails from accumulating dust. If I were just cutting aluminum, I would go with the setup you recommended. Thank you for all of the help, this is such a great forum with very knowledgable people.

Glad we can help. I also do a ton of FR4/G10 and carbon fiber work in milling custom FPV drone frames. I would highly suggest you look into some sort of dust collection system inline before your vacuum system as the swarf from composite milling will clog your vacuum filter very quickly and it is a pain to deal with when changing out filters. A good cyclonic dust system will do wonders if you plan to mill it on a large scale like we do. From vacuum resin infusing our own carbon panels to milling them out, we take great care to avoid the dust and the cyclonic system on the vacuum line has been one of the best things we did for carbon fiber dust control, that and of course having a fully enclosed milling system on the XC and our other two mills. If you have to dry cut carbon fiber panels, the cyclonic dust system is a life saver in the end.