Good evening all, I'm fairly new to CNC - I got a Lead 1010 about 2 weeks ago, haven't done any milling or CNC work previously. Got into it through school (taking an electrical controls class). I've cut a few wood projects in the past 2 weeks, nothing overly fancy. I've been running a 3D printed chain sprocket on another project, while attempting to source a proper, metal one. Tonight, that sprocket broke, and I'm really sick of printing them. McMaster Carr has them, but they want an arm and a leg for shipping. Since they have all the drawings available, I figured it would be fairly easy to cut one out, and I happen to have a chunk of 10mm 6061 aluminum sitting here. I'm running a 1.5kW spindle, and I've imported the DXF files into Carbide Create. Using the tools preloaded, selecting aluminum, gives 18,000 rpm and a set of feedrates. I can do 90% of the cut with a 1/4" bit, and the remainder with a 1/8" bit. I have both in upcut spiral, 2 flute, carbide. At the moment I have no dust collection, cooling mist, or air spray available on the machine. CC is saying 9 minutes for the 1/4" toolpath, and 3 minutes for the 1/8" toolpath - part is about 30mm x 30mm x 10mm. Since there's no good place to put a tab that won't be highly difficult to remove, I had planned on two-sided tape as well as clamping the aluminum down. At the tool change, I can also drive a screw down through the bore of the sprocket, as that will be cut fully, and the machine won't be going near there again. Am I missing anything major? Is it worth doing the toolchange, and using the 1/4" to clear the majority before cleaning up with the 1/8", or should I just do it all with the 1/8"? Is attempting aluminum at this point a bad idea? Appreciate any advice / insights!
I don't have a Lead Machine. But I'm a firm believer of trying. Maybe if you have time try a scrap piece of alum first and get it dialed in. In my opinion better to mill with the bigger end mill as much as you can. Recently I broke a 1/8 end mill trying to cut it all with it and was down waiting for new ones to arrive to finish the project. As far as holding my part down my process is securing the outside of the stock material first then bore, pocket and cut everything in the middle and then drive a few screws thru the middle for the part cut out. I have not tried double sided tape for part holding. Although double side tape wouldn't hurt. Sometimes a part if not held down in the right spots will bump it self loose. So friction on the spoil board side of the part is a good thing. I also made little clamps with 90degree notches in the ends out of 3/8in alum scrap to press hold part to the spoil board. I use sheet rock screws thru the clamps. Sheet rock screws are slender and semi strong and don't ruin the spoil board as much as other screws. I'm no expert just learning myself and having fun. OH! with Aluminum I have no oil or dust collections so I sit there with the shop vac vacuuming all the chips as they're cut and thrown out. hopefully rush of air helps cool the bit and keeps chips from being re cut. Even a ZRN endmill will melt alum to its self if there to much debris in the path being cut. EDIT- So I looked at the Lead 1010 machine. Do you really have 1.5kw spindle on there. With the weight and single alum ext across the X axis you might have some form of wobble and deflection from the spindle trying to cut alum. Just be cautious.
An option I would try, if there is room, is add two holes somewhere on the sprocket in your CAD software. Clamp down your piece, mill these holes first then screw it down and remove the clamps. Then there is no need for double sided tape. This is how I cut aluminum, although most aluminum parts I cut already have holes to be milled so I don't need to add any. That way I never have to clean up tabs.
Don't wait until the tool change- do the bore immediately after the face and then an M0 mandatory stop (not right on top of the part, learned that one the hard way) to insert the screw. You can cut aluminum dry but watch for deflection and make sure your CAM is cutting a full proper chip- low chip load will build up heat, and you'll get chip weld. It can happen real fast if you're not paying attention. Air blast would be preferable if you can rig a blowgun somewhere. Keep a vacuum or blowgun handy when you do the bore(s)- chips can't get up and out by themselves. Yes, just do 0.5mm stock to leave so you have some leeway in your tool diameter measurements and TLO probes. Probably not, as long as you don't overload the machine. Just don't expect the greatest surface finish of all time. While you have to cut a chip, you can't go too heavy on the chipload- 0.02mm/0.001" on the 1/8", maybe 0.07mm/0.003" on the 1/4". That's a guess though, look at what others are using on their gantry machines. Corey's concern about deflection is real. I was also going to suggest this. The holes/slots often found in gears and sprockets could be to your advantage here. Hard to tell, at 30mm diameter, if you'll have space though.
As Rob said you can cut aluminum dry. That is what I do. Every once in a while I may squirt some WD-40 into the slot to assist in cooling. To be honest, I do not know if it helps much. The router blows it across the surface and throughout the slot. There are those out there that have said it gives a better surface finish. I have not noticed much difference. I am getting a pretty good finish with a 1/4" two flute endmill both dry or with WD-40.
The only end mills I get what I'd call a "good" finish from are YG-1 Alu-Power 3 flute 45 degree high polish uncoated carbide. Cut like butter and leave a mirror face. They're not a bad price, just not one I have an easy time justifying for (for not too much longer!) primarily personal prototyping work. I use Rogue Systems end mills at the minute. They're cheap, they're good quality, and for those who care about that sort of thing, they're made in the US. I haven't tried Harvey, Niagara or Lakeshore yet though, but I doubt they're significantly better than Rogue except maybe in available options (since Harvey owns Helical and Micro100- I do have some Micro100 lathe tooling though, they're fantastic).
Feel free to send me some of those high helix three-fluters to, er, "test out" when I have M4 up and running.
Well, that was definitely a learning experience! Biggest one - I need a better location for my machine, where I can build a decent enclosure for it. I have aluminum slivers all over the basement right now. I originally went with the feedrates in Carbide Create; I compared them with GWizard, and found they were on the high end of the recommendations. So I ran the 1/4" roughing at 75% and the 1/8" at 50%, and I'm pretty impressed with the output. With a small bit of sanding, the sprocket is nearly identical to the purchased one I have. Definitely easier to tap the set screw hole in the aluminum than it was in the steel. In terms of deflection, I really have no idea at this point how you would measure it, but I can put all of my weight down onto the X axis beam, and there is no noticeable movement of the bit. If I grab the spindle, I can maybe get a few mm of movement out of the bit. I'm sure once I get into more precision work, I will have to re-evaluate, but for now it seems to be pretty good. Thanks for the boost of confidence; not sure I would have had the guts to try it without the feedback. Cheers!
Ah ok I just thought it was heavier. My Makita RT0701C spec says 3.9lbs and the Google'd info I found on the 1.5kw spindle was close to 7lbs
Probably water cooled. Perhaps also the difference between 3 bearing and 4 bearing, body/rotor length, etc. Not all China spindles are created equal.
This video came out a few hours ago and deals with the feed and speeds things we all need to know (-:
