We’re a newer team (Vector 8177 from Houston, Texas) facing a pretty monumental problem right now. We have a custom robot this year and have lots of metal and polycarbonate parts on the robot we want to CNC. We have an omio-x8 2200L usb, have complete control, know how to use it, and are all set on that front. The problem is that of actually fabricating. We didn’t purchase a bit cooler because we had no idea you needed one for CNCing aluminum, and after a couple days of bits breaking we realized we were probably undergoing chip welding. We don’t think we can buy/install/setup a mist cooler right now, and might have to resort to getting our parts fabricated by someone else if we can’t come up with a solution. We know the problem is the cooling and not leveling because setting everything slower and spraying wd-40 on the bit every 30 seconds resulted in no breakage. What do you guys recommend for a cooling solution that would be cheap and easy? Is an air hose attached to the spindle pointing at the bit outputting up to 100 psi sufficient (this option is available to us)? Are those aluminum bits that have a ‘coating’ on them requiring no cooling viable? And if so, for either one of those options, what inputs should we tweak to get a successful cut? We’re planning to cut 1/8" Al and 1/4" lexan/polycarbonate. Appreciate any help!
I highly recommend taking a look through this entire thread:
Generally speaking, pressurized air and a mister are the things that will give you the best results. Also, be sure to use single-flute carbide endmills.
What endmills and feeds & speeds are you using? It is possible to feed to slowly, which cause the tool to rub and heat up. You want the heat to be leaving with the chips, not building up in the tool.
A mister will definitely give you the best results, however it is possible to run with out one. We’ve been cutting sheet aluminum on our ShopBot up to 0.1" thick using 4mm single flute carbide end mill at 42ipm/0.002fpt, 21K rpm using an ~100 psi air blast and chip vacuum. We run 1/4" polycarbonate using the same end mill at 168ipm/0.008fpt, 21k rpm with just the chip vacuum. That being said, a mister is on our wish list once the router gets moved to it’s own room.
What size of bits are you using and what speeds and feeds and depth of cut are you using.
We have two machines that we use often.
In aluminum we usually use a 3/16 single flute upward spiral carbide bit. Feed rate at about 30 in/min and plunge at about 10 in/min. I have seen much higher numbers on here, but that is typically what we use and have had decent results. We only use about a .042 inch depth of cut. At least 3 passes on 1/8 inch and 6 on 1/4 inch.
We don’t have a mister as of yet either, but will spray a light coating of wd40 and then lightly blow some air near the bit when it is going. Might respray another coat on separate passes.
edit: forgot a zero in my depth of cut
Its not necessarily cooling; chip clearance is always a challenge on Aluminum. Poor clearance leads to re-cutting and then on to welding. High spiral end mills can help.
Avoid Aluminum containing bit coatings for working on Aluminum. IE: TiAlN. Non-Aluminum containing coatings should -help- stuff.
Yes, an air nozzle pointed at your cutting area will help you some. Throttle it back with an upstream valve, though. An open hole at 100 psi makes a LOT of noise. A small wobble piston compressor (like for an airbrush) can run into a 1/8" hole and makes a solid chip blower without making your ears bleed. Locline or a clone would be a good way to get it in there; you need to make sure that your air jet doesn’t make bit changing a pain and that it hits the right place.
We’ve been running our Omio (purchased last spring) all fall and season, without any major issues (no broken bits, but our first ever cut last summer we did have some chip welding). Like you, we don’t have a cooling system installed yet, but it is on our to-do list.
We’ve been using Tap Magic (https://www.amazon.com/dp/B07CMNTFRN) whenever cutting aluminum. We have a couple of small cans that we refill from the jug. Squirting it out over where you’re cutting can really help keep the cuts nice and clean, providing some consistent lubrication.
I’m working on pulling up the numbers we have for our bits, will update here once i get to them. 4mm, single flute bits purchased from Swyft Robotics - we got a pack of 10 from them, expecting to break some, so now we have 9 extra sitting in a drawer waiting for use in a future year 
Ok, here’s our cutting settings. For aluminum, 0.1" depth of cut (I should note we do fudge that with thinner material, and will do 1/8" wall on a single pass, plus most of what we do for the robot is Versatube at 0.1" or thinner wall thickness).
For polycarb, also a 0.1" depth of cut.
In both cases, we get a nice “tail” of shavings flying out behind the bit!
We occasionally had some issues with smaller end mills using our Omio X8, also with chip welding. We dialed back the spindle speed a bit, kept the depth of cut relatively shallow, and dialed back the feed rate and that all helped a lot, but what really did it was installing a 3D printed vac hood on the spindle and hooking it up to the shopvac. That cleared a lot of the chip and, unlike a blower system, didn’t spread chips all over the place.
I have good luck just using compressed air (10-20psi), sometimes spraying/wiping a little WD40 on the aluminum surface before starting. You can also use bandsaw blade wax or grease. Don’t be afraid to put a little on the tool as well.
Change your settings to run everything you can as single-pass/full DOC. This basically eliminates chip recut as a problem and spreads wear out over more of the router bit, letting them last longer.
For aluminum I use .001IPT, 24krpm, (and thus 20-24ipm feed with a 1-flute tool) at a DOC = tool diameter. I only use 1-flute tools in aluminum. Anything else has chip clearing and/or tool rubbing issues with my setup (and I suspect many others do as well).
Give this a shot.
Feeds and speeds have a large effect on your cutting experience. People often try to be too cautious when first using a machine which can cause poor tool life, tool fracture, excess noise and slower machine operation. The important values are “Spindle Speed” which is how fast your bit is turning in RPM. “Feed Rate” which is how fast your machine XYZ axis move in inches/min or mm/min. “Chip Load” which is how much material a cutting edge is removing in inches or mm. And of course the bit information (diameter and # of flutes). Some combination of this information can be used to calculate the missing bits of the information.
The place to start is finding manufacturers recommended specifications. For example if I use a bit from Amana tools I can find it on their website for example this bit. There is a tab called feeds and speeds and open the PDF.
here you can find some information on the bit as well as calculations at the bottom
I start by using the recommended chip load per tooth (0.003"-0.006" start on the safe side 0.003) and multiply it by the number of flutes my cutter has (1 flute) and multiply it by RPM which I can chose based on what I am comfortable with without going above max RPM if listed (I will chose 12000RPM). My calculation results in 36 inches per minute. The more comfortable you get the you may consider going to a higher chip load per tooth and or RPM if listed on spec sheet.
Depth of cut wont affect the chip welding issue but may affect tool fracture. A good place to start is same depth of cut as cutter diameter (1/4 bit cuts 1/4 deep). Softer materials such as soft wood may allow for deeper cuts while harder materials such as aluminum may require less.
Now why certain issues occur. If federate is too high, spindle speed too slow, depth of cut too high, then the chip load would be too big for the cutter, this could cause the bit to break, chatter which will make a vibrating noise and leave a poor surface finish and poor accuracy and this could create excessively large chips.
If federate is too low, spindle speed too high, then the chip load will be too low which means the cutter is having to cut much more then necessary for the operation. This causes excess wear and excess friction, can cause it to rub rather then cut which causes lots of friction, chip welding which eventually causes the bit to break since it can no longer cut, excess heat buildup from the friction which leads to chip welding, and lots of loud squealing noise. Also this is the most common problem people have.
here is a good chart to explain this.
What causes tool wear. Smaller chip loads means the cutter has to form a chip more often which causes excess wear. The cutter doesn’t really wear much more by taking bigger chips but can break if the chips are too big for the cutter. Also if a bit gets too hot then it can ruin a bit.
Why single flute bits. The reason people like single flute cutters for CNC routers is because it can run at half the feed rate of a 2 flute and 1/3rd the feed rate of 3 flute and so on which makes it easier to hit the manufacturers recommended chip loads without requiring as ridged or powerful a machine.
Why cooling. Be carful about using active cooling to fix feeds and speeds issues. I highly recommend ensuring feeds and speeds are tuned first and then using active cooling to allow for higher chip loads (within manufacturers spec), deeper cutting, better tool life, lower noise better surface finish. Chip clearing is also important more so for surface finish.
If I have made any mistakes please correct me. I will try to come back and edit it.
Here are a couple good videos on this topic as well.
Shapeoko Feeds & Speeds and Machining Tips! - YouTube
Speeds & Feeds Tutorial for CNC Machines! WW164 - YouTube
Thanks everyone for the speedy and invaluable input! We’re currently finishing up a piece of polycarbonate (this we can cut because no chip welding cooling issues) and will test out metal with the recommended feeds and speeds replied here, 3/16 non spiral (don’t have any spiral) single flute carbide bit, implementing a wd40 layer on top of the part and 100psi air hose aimed at the bit/metal contact point. As for what feeds and speeds we were using during the failures, I will have our machinist post them here asap. Also, after viewing the cheap yet effetive mist coolers posted here, we think we’ll slap one onto the next buylist. Thanks again for the advice, and I’ll update with how it goes!
Houston is a big city with a fair amount of industrial activity. You are likely to find someone in the are stocking the types of end mills you need. If you talk to them in the right way, you may be able to add a new sponsor 
Post some links to some short videos, we can tell you a LOT about how you are doing based only on sound of it cutting.
Heyo, 8177 Machinist here.
I wanted to be really conservative with our settings when cutting aluminum because
A - when i used a feeds and speeds calculator and used those settings, it snapped the bit(lack of cooling im assuming)
B - i’ve never used a cnc to machine metal before, so I didn’t know what to expect
Both scenarios were using a 1/8 single flute carbide endmill(straight, not spiral)
When running at about .01" doc, 15k rpm, 30 ipm, and 5 in/min plunge rate, it cut fine with regular wd40 spraying.
When running at the same settings but chaning the doc to .03," the bit snapped within a few passes.
After that I was frustrated enough that I decided to give up on aluminum for a few days and cut all our polycarb pieces first, as our mentor said he might be able to get a company to lazer cut our metal parts. I haven’t done more testing, but on friday or saturday I most likely will mess around with air blasting for cooling and different feeds and speeds.
Will take a video next time we cut, thanks!
15k rpm is SLOW for a router cutting aluminum. We run our 4mm(0.158 inch) single flute cutters at Max spindle speed of 24k and a high feedrate for us is 45ipm with WD-40 mist and airblasting the cutter for 0.090" 6061-T6. If we didn’t have air we’d probably cut that down to 15ipm. No oil mist but did have air, we would drip oil periodically and probably run around 20-25ipm. Air makes a HUGE difference and oil helps too.
Would you cut 3/8" Polycarb in one pass with a 4mm single flute endmill, or is that too much?
Also, straight flute is normally only used on wood in a hand router. You really want some spiral angle; helps chip clearance and reduces shock loading.
ah ok good to know. I only had it at 15k cause i wanted to generate as little heat as possible and i was under the thought process of lower rpm = less heat generated. Thanks!