Hey guys, we’re having some major difficulties with cutting aluminum on our CNC, and we’re hoping we could receive some advice on how to fix our problem.
Recently, when we try to cut aluminum on our CNC, the chips don’t really fly away, and instead bunch up, causing them to get in the way of the end mill during future passes. This especially happens during pocketing and profiling operations. We call this “melted butter”
We’ve tried a few feeds and speeds combinations, but here’s what we have right now:
-4mm 1 flute end mill (from thriftybot)
-20k rpm spindle speed
-20 ipm cutting feedrate
-0.03 inch pass depth
-Aluminum 6061 (normally either 1/4" or 1/8" thick)
Notably, we don’t have a constant stream of coolant shooting at the end mill; we only have an air hose that somewhat helps with cooling and chip removal. The melted butter constantly gets in the way of the end mills during passes and sometimes breaks the end mill.
Can anyone help us solve our problem? If any more details are necessary, I’d be more than happy to provide any information. Thanks!
Edit: I run the same .001ipt all day and half the night without coolant or lubricant, only air, and go up to tool diameter in DOC, all on a floppier machine than you have.
I made the first few thousand grasshopper nuts with one 4mm TTB bit going full depth in the .09 5052 h32 aluminum with just air.
Don’t think of the air hose as providing “cooling” (it isn’t doing so in any meaningful way).
Do think of it as providing chip removal [in addition to the geometry of the cutter]. Accordingly, don’t position it in the next room over like in the photo, but instead position it much closer to the bit [and maybe more downward-directed] to help it blast the chips out.
That’s a fair depth of cut for slotting on a machine of that class. I would be inclined to try a lower DoC and a higher feed rate to try to get a chip rather than dust.
We had the same problem with the same bit this weekend, but solved it completely with a squirt bottle of Isopropyl and soap. We’re running 22000RPM 60ipm .060”doc.
I think from the look of your metal you have too fast of a spindle speed and too slow of a feed speed. Depth of 0.03 should be fine but sometimes we step back to 0.025. Our feed with that exact bit works at 32 or 36 ipm with 10,000 RPM. I think you are melting the aluminum and it will get stuck in the flute or make this mess.
The other thing to check and double check is the bit in the collet. We had replaced a bit and right away all aluminum cuts looked just like yours – found out the collet was not fully seated in the spindle and that the bit was not perfectly straight. A little wobble makes a mess.
Alternatively use a small amount of WD-40. That work very very well but is harder to clean up. Put some at the tip every few seconds until you get a channel then when you get a channel, put some ahead of the cut and vacuum clear behind it. Even if you don’t get chips flying, this slurry will make your cuts clean. Before we got the mister/air WD-40 worked very well and we still use that if we are making a deep 2D contour where the sprayer just can’t get into the slot. We just carved out a complex 3x11" long piece from 5/8" thick plate with a 4mm bit on Friday using mostly WD40 in front of the bit and vacuum behind–took 90 minutes but was beautiful.
Feel free to message me directly if you want or add more discussion questions here.
Looks like you’re running an Omio (or something similar)? Your RPM looks good but you might want to increase your feedrate (somewhere between 50-60ipm) and decrease your depth of cut. Better to take a bunch of shallow cuts quickly when your working at those RPMs and a small endmill.
We’ve used some feeds and speeds that someone posted in an Omio thread a while back, but even with those we have issues cutting aluminum with anything smaller than a 1/4" endmill to the point where we try to avoid it if at all possible.
We don’t even run our 1/4" endmills this deep. If we tried this on a 1/8" endmill it would snap immediately, even if it was brand new.
When we have broken an endmill, by far the most common cause was the tool slipping in the collet, causing us to go over 1x DoC and it snapping off. Running slower doesn’t always mean you will have longer tool life. There’s less material removal so the tool ends up rubbing and building up heat in the tool itself rather than in the chips.
Run faster. Go 60-70 IPM. With a 30 thou depth of cut it’ll be barely any load on the tool. Hear builds up the longer the tool is in the area - the heat can’t build up if the tool isn’t in the area for long.
You have too much stickout, too much flute length, or both. Or something really wonky with your spindle. Whatever it is, I strongly encourage you to diagnose it properly, you will make that machine dramatically more productive.
Cutting shallow passes wears just one small fraction of the tool. Cutting .06 instead of .03 will double how much material that tool gets through in its life. Going .12 quadruples it.
Going full DOC (thru the material) ensures you never recut chips, avoiding the most problematic part of routing aluminum.
You definitely want to keep from recutting chips. In addition to air on the cutter, I use either a chop vac and or a hand held air nozzle to keep the table clear. especially on longer cuts.
Just keep clear of the over travel limit switches.
Looks like you either have a tool slippage problem, or are cutting way too far through the stock into the spoil. We typically only cut .010-.015" through the bottom of our stock. That spoil material is still being cut by the end mill, so excessive cut through can clog the flutes with MDF before if even gets a chance to evacuate the aluminum. Using coolant can also cause the MDF to turn into a sticky paste in your flutes, making chip extraction even more challenging.
thanks for the replies everyone - i think this has been a recent development, at least when i was running this machine a few years ago we didn’t see any of these issues. has anyone else used thirftybot endmills recently and gotten decreased performance out of them? they were my go to but i’ve observed that they’ve been wearing faster than i remember.
I would run it dry, but increase your air evacuation if you can. The Up Cut End Mill would force the chip to come out. You should see chips like tiny little rice grain. You would leave a little burr up top, so run secondary chamfering to clean up.
What was your Width of Cut? Try to get .001"-.002" chip load.
Better clamping. Use mechanical clamping if you can.
The 1/8in bit, with 0.86in flutes (22mm), is about 8% as stiff as a 4mm diameter x 12mm flute TTB bit.
It is about 2.5% as stiff as an 1/8in x 1/4in flute bit from McMaster: 3317A21 (pretty sure this is Onsrund brand).
I have used those same bits from Amazon. They are no good for aluminum simply because they are not rigid enough. Try TTB bits if you have metric collets. Some options from Amazon in English sizes that I have liked include:
(These do okay in aluminum, but not as good as a TTB 4mm bit or the 1/4 DOC Onsrund but)
