Ok, so I gather that i'm not the first to want to use my workbee to cut something in aluminum - and i've read tons of posts about it before my experimentaiton started, but they all tend to say slightly different things. Well, i've gone at it, and decided to experiment a bit, and now i hit problems, and would love some fresh eyes and suggestions. I've got a nice 8mm chunk of 5083 cast and milled sheet. And I drew up a little clamp in fusion, as i thought that would be a good place to learn. it's a 50x75 workbee with a 500w china spindle doing about 12.000rpm at max. The fist clamp I cut out at 12000rpm with 1000mm/min at 0.25mm depth of cut as max using a three flute 4mm endmill, and my compressor to keep it free of chips. That worked quite well. So i guess i could just stick with that. But... I also did a pass with a single flute endmill, which did not leave a particular nice surface finish, so i gave that up as a bad idea. (probably my single flute endmill was too soft (china)). then i increased my depth of cut to 0.5mm and things started to go wrong. first i gunked up my endmill. i figured it couldn't get rid of the chips fast enough, so i thought - hah, i'll pick a two flute endmill, as there will be more room for the chips to get out. (still with my compressor blowing air at it while cutting). That just ended up in a broken endmill. And this is where i kind of get a bit of a question mark. with the same settings, the twoflute essentially burried itself.. I don't know if you can really see it, but essentially the bit dug itself into a hole and gummed up. that wasn't expected. does that mean that my X and X axis is essentially too soft to keep the bit from pulling the whole machine deeper into the material? Also the slope i did with a R2 4mm ball endmill with a stepdown of 0,1mm - i don't get a particularly smooth finish, and i'm thinking it's probably rubbing too. I've just bought a mister, that i want to mount and see if that makes things better - any suggestions on oil/mixture for that? Also - any good advice would be very welcome
You haven't picked the best alloy, 5083 has poor machinability ;- Aluminium Alloy - Commercial Alloy - 5083 - '0' - H111 Sheet and Plate Using 6082 T6 I have had success using 10~12.5 K rpm, 500 mm/min, and 0.2~0.5 mm doc. I think I could increase the feedrate on my machine, but that depends on the rigidity of your machine. Using alcohol (isopropyl or meths) as a coolant helped a lot. I found anything oily made things worse - clearing the chips is essential. I suspect chips welding themselves to the cutting edge of the bit is a major cause of your problems. Single or two flute bits will give better results than three flutes. I use (cheap Chinese from ebay) 3 mm single flute spiral and (even cheaper) 6 mm two flute straight - actually router bits - the angles on the cutting edge of a router bit are well suited to cutting aluminium. Alex.
Aha! - i had it recommended by a local maker-3d print and hobby cnc shop. i guess that it'll be great for the little clamps i'm making as it's strong, but fair enough, it's not the easiest alu to machine. what would be the best way of solving the problem of chips welding themselves to the cutting edge? Coolant? /Kristoffer
Coolant will certainly help a lot. When you have used up (or decide to give up on) your 5083 look for some 60xx series alloy - 6061 or 6082. Looking at your pic of the bit it appears to have quite a lot of aluminium welded to it, my first attempts with aluminium had the same issues (no idea what the alloy was) and the only way I managed to cut it (with disappointing quality) was pausing frequently and removing the chips that had welded themselves to the bit - I don't recommend this! . Alex.
Diamond Carbon Sharkbits from openbuildspartstore.com - the coating prevents welding/gumming of the Alu, and yes, coolant helps too.
There's a always a salesman around ;-) That sounds like a good shot. i've just added my mister, and will give some coolant a shot today. but probably some fresh bits are in order. I've noticed that once the bits start gumming up, they just seem to become stickier and stickier...
Yes - as soon as you get aluminium welded to the cutting edge it stops cutting and rubs instead - more heat & more melted aluminium. Alex.
Another reason you may have "plunged and buried" the endmill is that the collet was not tight enough. This has happened to me. My 1/4" 2 flute endmill started out at 0.8mm DOC in some 6061 aluminum and soon was plowing through the full 6.5 mm thick plate and the spoil board beneath. Knowing it could do this by accident, it made me confident I could increase the aggressiveness of my cuts.
It's a dance. But my recommendation is with Peter Van Der Walt, any end mill that is ZRN coated or Sharkbits diamond like coated endmill. 98% of my problems stopped when I got a ZRN coated 2 flute 1/4in and 1/8th end mills. Also I have found if you use a sheetrock screw you clean the end mill of melted aluminum. Start at the shank end keep the screw tip in the middle of the groove and follow the flute down to the tip, you can "dig and peel" to the tip you can remove the aluminum. Do not start at the tip and try to dig it out. You can damage the cutting edge. And as you mill the piece you can utilize your tool path to cut intermittently is the best. Like Trocidial style milling. I just cut a part out 9.525mm thick alum 3mm DOC with a optimal load of 1mm with Adaptive Clearing in F360. It's extra work in drawing but this is what I drew on my part to be able to get the end mill to oscillate. The end mill "cuts then rests". For the edge that's to left on 1/4 end mill I give it about 10mm gap. My settings are probably nil cause I have a different machine build. But Just a thought for you cause I tend to keep my RPM in the same range as your 500w spindle. As I'm cutting and with the vacuum up close removing the chips if I notice the some chips are still sticking to the sidewalls of part I slow down the spindle/router till I notice 98% to none of the chips are sticking. My Makita is probably close to 12000rpm. I started out at 2 on the dial and slowed it down to about 3/4 between 1 and 2 and my router lowest rpm is supposedly 10000rpm. I guess I should invest into something that can read rpm of router but for now its sight and hearing. This did a 20min job with no problems. And your part you are milling looks good I like the champfer and your solution for holding your part. Can you get a full pic on how you are holding that plate down? Thanks! machine
Yes. I did check that, as I did have a similar experience half a year ago. And sometimes it's quite extraordinary what your machine will do when you don't ask it to
I can't believe how big a difference it makes. After i got the mister working with some spirit and compressed air, I rand out of 4mm endmills for alu (**** happens), and had to default to a cheap 2flute chinese HSS endmill that i'd normally use for wood. And look at this: No gumming up, much nicer finish than the previous runs (the program is largely unchanged, except i added a threaded hole). machine ran beautifully. though i did have both the mister and the vac running at the same time. One question remains. How do i get rid of the lines where it goes up and down when making the tabs? (is chosing rectangular tabs enough? - spotted the option in fusion after doing the clamp.) Thanks for all the helpful suggestions. Best /Kristoffer
I use blue masking tape and superglue to hold the material down - don't need tabs then as long as you make sure any bits that might be cut out or off the sheet have tape and superglue holding them. If using a large sheet of material I often add a couple of clamps away from the part being cut as "insurance". Alex.
Thanks for the pic I like the setup. I have been using only sheet rock screws and various chunks of aluminum to hold down work to wood spoil board. But I am gravitating to some form of bed with bolt holes.The tabs on your setup is low profile and a perfect idea. Thanks! Thanks for the idea.I like the idea of tabs some times I am cutting a small piece that I trued up one edge or a 90 degree corner. It's nice to have a system that is squared to the gantry throw part in and clamp, zero and cut. I think I spend more time truing the part to the machine to be able to utilize all materials trying not to create to much waste. Although I am curious how well the glue holds the parts and bits that need to be removed down. Have you ever had any parts break out from the glue and fly out or move jam against the end mill? Currently when I am cutting and I have a middle piece that's gonna be loose once done, and needs to be removed. I have the vacuum ready to suck it away from the end mill as quick as possible. The one time I neglected to use the vacuum to get it out of there it lodged crooked in the whole broke the end mill.
Not had problems with loose bits flying around, but you do need to anticipate the possibility and make sure that any bits that might have both masking tape and superglue to hold them down. Cutting oil (which I used for cutting mild steel) can soften the adhesive on the masking tape, but on the (one) job I have done it was only at the very edge - masking tape did not come loose. Alcohol (used with aluminium) didn't seem to affect the masking tape at all, but I haven't set up my mister yet, so was dripping meths just ahead of the bit rather than spraying it around. Alex.
