Our team received a 3-axis CNC router from our sponsor last September, and we’ve been trying to use it to cut aluminum boards. After a year of trials and errors, we’re still facing challenges as the milling cutter keeps breaking, forcing us to frequently switch cutters. I suspect there may be issues with our setup, but none of us have experience with routers, so we’re seeking guidance from the forum.
Specifically, our CNC router operates on 220V with a maximum power of 2.2 kW and features a water spraying system, which we’re currently using to cool the cutter. We’re working with a 3.17 mm cutter, set at a rotation speed of about 20,000 rpm and a feed rate of 0.1 mm while cutting the bumper connector for our robot.
Should we adjust any of these parameters?
Additionally, we’re using G-code generated by the manufacturer’s software. Should we fine-tune it ourselves to optimize performance? I also noticed various types of milling cutters available. Should we consider changing the cutter based on different cutting functions, such as drilling or profiling, or will the 3.17 mm cutter suffice for our needs?
Also, are there any other things we need to pay attention to when cutting aluminum boards?
Can you send a picture of the machine or a model number?
Does “feed rate of 0.1mm” mean 0.1mm per rotation? That is very fast for a 3.17mm cutter, 0.03 to 0.05mm/rev is more common. Also, a 4mm endmill is a lot stronger and can be pushed at 0.05 to 0.1mm/rev.
How deep is the cut? What is the final feedate? Are you using adaptive clearing?
That’s what I was thinking was going on, cutter being just a hair small and being pushed too fast in feed rate. It’s not the heat that’s killing it, it’s the force.
As far as changing the cutter based on what you’re doing–that generally isn’t necessary for a router.
Try using a single-flute cutter for aluminum. Run it fast, at least 18k RPM.
Chip load is the amount of material the cutter removes with each rotation of each flute. You should be able to enter spindle speed and chip load into your CAM software, and it will give you a feed rate.
For a 1/8in. cutter use a chip load of .003. These are starting numbers that should work well enough.
Make sure your workpiece is held down to the table well (e.g., with clamps) and it isn’t moving around. To start, don’t take more than 1/2 the diameter of your cutter for the depth of cut.
We have had great success with them. They will last a whole season (unless you run them into hold-down screws)
For cutting, I do 24k RPM (a bit high maybe, but it’s hard to change the spindle speed on our setup), and 30IPM in aluminum. We mainly cut .08" - .125" (2mm-3mm). You can go faster with bigger endmills, like the 4mm or 5mm endmills
For 5mm thick aluminum, I would do 2-3 passes. Cut 2mm deep each time (in Fusion 360, this is the “multiple depths” option on the 4th tab)
Make sure you spray a healthy amount of cutting fluid, whether it be alcohol, WD-40, loctite cutting fluid, tap magic, something. We do WD-40. Aluminum is very “gummy” and will stick to the tool when heated up or cut. You need something to prevent that from happening. I also suggest maybe getting a tool mister like the FogBuster, but a student with a spray bottle will also work.
Also - make sure you hold your parts down well. You might want to get a long stick to hold the pieces you cut off down. Sometimes the parts move and jam the cutter and break it
I have had tabs give up (part of this is tab setup being too wimpy) but the long stick should be a backup you have ready to go in case the tabs fail. Better to hold it down manually (with the stick , not your hands) while the job finishes instead of ruining the entire part/breaking a bit
We’ve also had problems over the years with cutting aluminum on our router (Omio X8) using small bits (1/8" in our case, very similar to 3.17mm), however we also don’t have the benefit of mist/flood coolant on ours.
As others have pointed out, there’s not enough information here.
There’s a few things to consider when Milling:
Endmill Diameter
Number of Flutes
Feedrate
RPM
Depth of Cut
Other machine-specific factors like power, rigidity, and coolant
Length of the Endmill
The first five items there all factor into “chip loading” which I’ll go into below. While you can’t control the specs of your machine, it is worth considering the length of your endmill. If you’re only cutting through 1/8" thick aluminum, but you’re using a 1" long endmill, you’re more likely to experience “chatter” which can lead to broken bits. While not always practical, it’s preferable to always use the shortest endmill possible for a given job.
As a bit of an aside, most coolant mist/flood systems I’ve seen are not intended to run with just straight water, they generally recommend a coolant mix to help reduce corrosion of the machine and assist with lubrication of the cutter. I noticed you used the term “water” so I wasn’t sure if you meant that literally or not.
In general, we run the following settings for our 1/8" endmills on our router for cutting aluminum:
This may require some trial and error for you, but in general it seems like keeping the feedrate and RPM high and reducing depth of cut as needed is the preferable way to dial in cutting with small endmills. That said, I do occasionally have to turn the feedrate down too when doing tight or deep pocketing operations since flex in the endmill may cause the pocket to be undersized if you go too fast.
Another thing we sometimes run into in our software is that when running pocketing operations it defaults to a very aggressive step-over. In general, your max step-over (how far horizontally the endmill cuts into the material each pass) should be <1/2 the diameter of the endmill, otherwise you risk “plowing”. Sometimes plowing is necessary (particularly for contour operations), but when possible, it’s preferable to do it with a larger diameter (and thus stronger) endmill.
Software depends a bit. Since we use Autodesk Inventor for CAD, we try to do most of our CAM (Gcode) in Inventor CAM as long as it has an applicable post-process profile for the machine in question.
If you are using the manufacturers software, on the one hand I hesitate to change default settings, but on the other hand it’s worth considering what your particular machine was marketed as. If it was sold as a router for primarily cutting wood, the defaults may not be applicable for aluminum (Inventor CAM seems to have most of its defaults for cutting Steel, so we have to fight that occasionally). It’s also possible if the router was sold as a wood/engraving router, the manufacturers software may sometimes lack advanced features you’d see in other industrial CAM software.
As to types of cutters, there’s a few things to note here. For milling operations we use single-flute flat endmills almost exclusively (or two flute if absolutely necessary, since single flute cutters have a somewhat limited selection). It’s worth noting that flat endmills are NOT optimized for drilling operations, so when possible we either use “pocket” operations with spiral ramp downs to “drill doles”, or just use a literal drill bit for drilling operations (incidentally, we have a set of 3-flute drills we got that are great for holding a center). Alternatively, you can also sometimes use ball-end mills for both drilling and milling, but we generally find them more hassle than they’re worth since you have to account for the radius in your pocket operations.
In general, we use 1/8" and 1/4" diameter single flute endmills for most of the polycarbonate and aluminum machining we do on our router (though their metric equivalents should be fine too). We do still break them occasionally, but they’re relatively cheap to replace so we try to keep a bunch on hand. Keep in mind that endmills, like all tools, do have a finite lifespan, even when you are using them correctly.
Make sure you’re getting 6061 aluminum and not 6063 aluminum, and buy from a reputable source if possible. 6063 aluminum is significantly more “gummy” and harder to machine. Some suppliers may mislabel 6063 as 6061 (either intentionally or out of ignorance) because 6063 is generally cheaper than 6061.
As multiple posters have mentioned, change to at least a 4mm diameter flat endmill. The resistance to breakage when going from 1/8" (3.17mm) to 4mm is much larger than you might guess it would be.
Make sure that you are using a single-flute endmill. This allows you to get feed rates in aluminum on hobby/prosumer machines running router spindle RPMs that cut chips rather than rub and create heat.
Bare carbide endmills are fine for cutting aluminum, especially if you mist a micro-lubricant. If you get coated endmills, don’t get a coating that has aluminum (Al) in the formula for cutting aluminum. Diamond coatings can be helpful and TiCN is OK. Getting cheaper bare carbide and changing them out more frequently may be a better strategy.
If you are using a single-flute endmill, you won’t need to worry about whether your software specifies the “feed rate” in feed per tooth or feed per revolution. They will be the same. Most software uses feed per tooth and needs to know the number of teeth on the cutter. Advice here of running a 4mm single-flute endmill at 0.05 - 0.1 mm/tooth is good. There was mention of running a 1/8" endmill (3.17mm) at 0.003 in/tooth (0.076 mm/tooth). This is a bit fast in my experience for 1/8". It might be possible in some cases, but if I had to run a 1/8" endmill, I’d wouldn’t start any higher than 0.05 mm/tooth.
I’m guessing this is a mist sprayer and not a flood sprayer since you are taking about a router. I’ve never tried to mist water with a router, but I expect that wouldn’t work well. You should be spraying a micro-lubricant to help keep heat generation down and keep chips from sticking to the cutter or the material. If you don’t have something like Kool Mist or MagLube, you might be better off just using the sprayer air blast to evacuate chips rather than spraying plain water (if you are indeed spraying plain water). The value of a mister on a router in order is 1) physically evacuate the chips, 2) lubricate sticky aluminum, 3) cool the cutter.
You did not mention the depth of cut you were trying. If you are slot cutting (cutting a part out of a sheet), you should be able to cut 5mm material with two equal-depth passes using a 4mm cutter. If you are using a 1/8" cutter (or want to start conservatively with a 4mm cutter), you may need to make that 3 equal-depth passes on 5mm. If you are clearing and cutting sidewalls, you could go full-depth, but limit your cutter stepover. You might try 20% stepover to start for full-depth clearing on 5mm and adjust as you see how it performs.
If possible in your software, ramping in cuts for slotting is a good practice to help reduce cutter breakage. Something like a 5-7 degree ramp angle works well.
No. The software has all the needed optimizations. Focus on providing good inputs to the software including cutter diameter and teeth, RPM, feed rate, depth-of-cut, ramping, and possibly other inputs that your software may provide.
The type of aluminum matters too, some are very gummy and really doesn’t work well with the router. We only cut 6061 and that seems to work pretty good. We use the thriftybot bits recommended above as well.
we’ve also used the thriftybot endmills in both 4mm and 1/8in and they work great. Would also recommend tabs and for workholding besides that we use double stick tape on our big CNC router (which I personally don’t think is enough but has proven otherwise) and on our omio we used to use regular wood screws into our spoil-board but I believe now we just use the tape.
A lot of people are recommending 4mm endmills, but depending on how small the holes you need are, you may be able to use 3/16" or 5mm endmills and cut even faster. 3/16" and 5mm are our standard cutters and we only get out the smaller ones when we need to use non-standard small fasteners.
Ah, by holding down with the stick, I really mean the cut out parts that aren’t part of the robot. The robot parts get held down with several screws into the spoilboard
I drill holes first, add 2+ screws to every part, then cut the internal and external geometry
