Any with advice on settings that worked for you when machining Brass (& Copper, if you have it) on MPCNC?
I have destroyed 7x 1/8" single-flute endmills from V1 so far on this and I’m in need of other peoples input where they’ve had success with Brass.
If you share your settings, please can you share with me your successful settings for both (a) 1/8" endmills & (b) 1/16" endmills using the following format (+ any other info you can share on top of this):
The endmills you linked are the good ones, always been sharp for me, and I’ve jammed them up in aluminum without breaking.
Brass is a good bit harder than aluminum, but I also cut a little bit of steel on my very VERY small burly, but that was all adaptive cutting. I never messed with pocketing and i never got profile cutting to be comfortable.
That said, it looks like your chip/tooth is on the low side. I would bump that up to at least 635mm/min for a single flute.
With brass hardness, you might also try a 2 or 3 flute mill. The single flute hits the material once a rev, so have having more flutes might even out the loading. Instead of bang bang bang, if that makes sense. Same way a v8 runs more smoothly than an i4, if you’re OK with imperfect analogies. Plus, with more flutes they are usually shallower (which is what we DON’T want with aluminum) and that translates into a larger core and more stiffness (although I think the endmill you linked has a large core for a single flute already, best case single flute, imo). You may have to reduce your stepover for this strategy.
And if the job will support a larger endmill, definitely get a larger endmill.
Well, i work in inches, so double check my math, but I haven’t had good results on anything at less than 0.001"/tooth. So I’m figuring 25krpm*0.001=25ipm=635mm/min.
2 flutes, you might want to double it (or so).
On top of that, as you go below 50% stepover, the actual chipload gets smaller than the calculated chipload(called chip thinning) so it doesn’t usually hurt to bump the speed up if you aren’t taking big stepovers. Light stepover+low feed rate+high spindle speed = rubbing->heat->dulling-> breakage.
This is why pro mills run so danged fast for high efficiency milling : small stepover, huge flute count…600ipm😬
All that said, it’s just my experience on my machines, and none of it includes brass specifically. Good luck!
What are the main formula’s that you use? I’m foggy on what mathematical formulas to use in practice when deciding feeds/speeds and anything I would need to calculate in theory.
The best practice is to test, test, test. Each machine is different. You can adjust the speeds, but also the strategy. Things like taking multiple finishing passes, or trochoidal milling, or peeling the material with more depth and small stepover.
I was only suggesting you search through some posts on aluminum. You will find more stories than with brass.
Most of us can’t adjust rpm very precisely, so most of the formulas we can use in cnc calcs aren’t particularly helpful.
I think it IS helpful to have a handle on the minimum chipload to combat rubbing (as above), but the first limitation on the mpcnc is (i think) rigidity, even before the nema 17s run out of power. As soon as the tool moves out of the calculated path, even a little, most of those calcs won’t have the same results as what your machine is actually doing and aren’t particularly useful.
Its not a nice answer, but there really is no good way to predict what’s going to work on your machine. Variations in size, printing, plastics, even bolt tightness can make a huge difference in how rigid your machine is. So far I’ve built a vanilla burly, a teeny tiny burly, a lowrider 2, a 2’x4’ primo, a 20"x24" primo, and I’ve assembled a 3’x6’ burly waiting on room for a table to set up. The performance envelope is different for each one, and needed testing to even get woods right.
I would think brass would machine easier than aluminum, because it doesn’t harden/gall the same.
On my small manual lathe cutting aluminum I have had to jam the tool in relatively hard to punch through the skin formed by a previous cutting operation, but with brass it is much more uniform. I’m not sure if it is exactly the same as work hardening but it definitely makes a difference. Also brass doesn’t tend to stick to the tool like aluminum does.
Bulk material strength and hardness will be a factor but maybe less important than you might think. E.g. stainless vs. cast iron are worlds apart in machinability.
FYI Everybody - the problem turned out to be lack of rigidity in the stock.
The double-sided sticky tape was trash on the MDF spoilboard. Carpet tape solved the problem and my results have been absolute perfection for the past 5 test cuts I did, even at the most demanding settings I’ve done so far. No Chatter, absolutely crisp edges and valleys of cuts. Just perfection.
Now I know what the problem is, I’m devising a removable spoil board for machining metals where I:
stick a plate of aluminium to the removable spoilboard permanently using the carpet tape, and then
using the double-sided sticky tape, stick my metal stock to the aluminium ‘spoil board’ surface (coz the double sided tape sticks great to polished aluminium stock, but will be easier to separate than the carpet tape after finish cutting).
Wish me luck, coz now my MPCNC has decided it doesn’t want to turn on anymore… lmfao.
Can’t believe I never asked how you were holding it down. I fix a piece of mdf to my spoilboard with locating pins, then surface the mdf. After screwing the aluminum to that, i can remove the entire shebang and also put it back where it belongs and bobs your uncle.
