I have a Shapeoko 4 xxl and a 5 pro.
I am using the Makita RT0701C Router and running it at level 6 - or 30,000rpm (highest rpm setting)
I am using an Amana HSS1630 2Flute Upcut 1/8" bit - 1/4" shaft.
I’m cutting 1/4" thick 5052 Aluminum.
Running @ Feed Rate of 20.
Each pass 0.025"
The issue is that occasionally (approx. 10-20% of the projects) the aluminum will (apparently) weld to the tip of the bit. When this happens - it ruins the cut (and part) and usually breaks the bit. Any recommendations on proper feed rate and/or RPM speed change?
TLDR: single-flute tooling, suitable coating, adjust feeds and speeds to take a cut/chip, not rub, if possible, ramp in, if possible, adaptive/trochoidal toolpaths.
Also you should check out the manufacturer recommended feeds and speeds for your tool:
Right off the bat it looks like that tool is only rated for 18,000 rpm?
Beyond that, you’re likely spinning the tool waaaaay too fast for that feed rate.
Feeds and speeds are annoying to calculate at first but it’s definitely worth your time if you plan on cutting any metals.
Specifically, I’d recommend you calculate your current chip load per tooth with the settings you are running. Conveniently, amana provides the formulas in their recommended feeds and speeds pdf
Compare your current chip load to the recommended. My guess is your current chip load is absolutely tiny compared to what it should be.
I see several things. First, increase your feed rate to at least 60 IPM or decrease your RPM to 10,000. That will put your chipload at 0.001" per tooth which is about the minimum I would recommend. You can do a combination of both. For example, 40 IPM and 20,000 RPM would also give the same result with that tool. The math to figure out your chipload is IPM / RPM / # of flutes.
Second, make sure you are fully clearing chips with either dust collection or air blast. Recutting chips will very quickly cause issues. Especially with 5052.
Third, consider using 6061 instead of 5052. The softer the aluminum is, the harder it is to cut cleanly. It can be done, it is just less forgiving.
Fourth, as @WillAdams says, consider using a single flute cutter and avoid slotting tool paths.
All of these things are just guidelines. There are reasons to not follow them, it just decreases your margin for error.
A - 5000 series is REALLY gummy and has a very narrow range of chip load that it likes. If you can, switch to 6000 series like 6061. It is alloyed to be MUCH easier to machine than 5000 series that is alloyed for bendability. The only reason to use 5000 series if if it needs to be bent after.
B - Get a single flute. With 1/8" a 2 flute is still workable, but the feedrate that works gets narrower, again, especially in 5000 series. In 6061, a 2 flute would still work great.
B - Bring the RPM of the router down. You want 16,000 max.
C - At least triple your feedrate. Seriously. It sounds counter-intuitive, but chip welding is the result of the metal melting instead of making chips. You want the feed to be high enough in relation to the RPM that is makes nice chips that carry that heat away from the cut. Especially in 5000 series aluminum, you want minimum of 0.002" chipload. At 16,000 RPM with a 2 flute, that is 75 IPM.
D - If you can, get at least air-blast on the cut.
E - Serioulsy, 5000 series is about worst case scenario for milling. Only use if absolutely necessary. I’ve cut in on a Shapeoko Pro, but only because it was a box that was being bent afterwards. I broke 2 endmills before I figured out it was 5000 series and I needed to get out the single flute and hall rear-end.
I cut much deeper most of the time. 0.025" is more on the conservative side in my experience. Generally 1/4 of the endmill diameter for a depth of cut is really safe. But if you’re going to back off of any parameter, keep the feedrate higher and reduce depth if you run into issues.
What you are doing with the aluminum cutting at such a high spindle speed and a slow feed rate is melting the aluminum instead of cutting it. As many people of said in here, chip load is important enough to be aware of so that you are getting the proper cut on the aluminum and you are dispersing heat properly. Cutting too slow while spinning too fast is more like welding aluminum with your cutter instead of cutting it. Vacating chips out of a cut is also important because the chips left in a slot cut will be cut again when the tool comes back around to the cut. On your machines liquid cool and removal is not feasible, but air assist is.
Slow your spindle down and feed it faster for cut the aluminum instead of melting the aluminum in a cut. There are great advices given up above and taking note of them all will help you cut aluminum better and more convenient. Again, material buildup on a cutter is signs of too fast of speed verses too slow of feed rate, aka welding instead of chipping.
Thanks Again Everyone - I think we are figuring this out, new question:
using the 1/4" HSS1636 for pocket cutting, rpm / feed rate / Depth of Cut? Same or Different?
