How does one decide depth of cut in aluminum to take? I googled a few questions about it nothing is sticking or apparent thought I would ask here. I Know my spindle is on the small side but i have been able to pocket and bore holes pretty good. its the part cut out and slotting I guess. I am thinking rule of thumb kind of info.IF you had my machine what would be max cut to take? Thanks! 500w spindle nema 23 Ball screws 8mm
Theoretically? Spindle power relates to volume of material removal per minute. Given that number, a chipload per tooth (which, depending on SFM/RPM, determines feed rate), and a radial depth of cut without tool deflection, you have a fairly narrow band of axial engagement to hit your removal volume target. In practice? Play with radial and axial engagements until your machine sounds happy and/or you stop breaking tools. Lubrication/coolant and chip thinning come into play here too, since aluminum likes to weld itself to the tool. Your machine might prefer wide shallow cuts or it might prefer deep light cuts, who knows. No extrusion machine, especially at 500W, is going to like wide deep cuts, I guarantee that.
I've never gotten shallow slots to work without welding aluminum to the bit, my machine isn't stiff enough to push through at low RPM. With trochoidal I've been able to do 6+ mm depth. In practice I run about 4.5mm DOC (clears chips better, 1/2" 6061 in 3 passes, I do 1/4" in two 3.3mm passes) 1000-1200mm/min feed with trochoidal % stepover of 4.5 and a slot width of 50% so a 1/8" bit makes a 3/16" slot. No, its not fast or something I would want to do every day to my belted Ox but i can setup, start and walk away from hour long jobs without blowing chips or using any coolant. Cheers Gary
Well I agree I have a narrow margin with a this spindle. I had thought i figured out the speed and the depth of cut. But pocketing and boring are different then the constant cutting. SO I have one more job to do on this part cut it out. But i am thinking i might removed this part before I dmg it and practive on a piece of scrap and tear in too with slotting or try the trachodail trick cutting whole part and speed Thanks!
I cut .156" to .188" wide slots in aluminum pretty frequently. I use a 1/8" HSS single flute bit & usually cut in about .025" deep passes, usually to about .125" total depth but I've cut deeper. Usually my slots are too narrow to use trochiodal / adaptive milling so I just profile around the slot. On a few occasions I've been able to adaptive mill & it's nice - I can cut the full slot depth in one or two passes. I'm using the Dewalt DWP611 router at 21000 RPM. I cut dry & usually make a fixture that's flush to zero so I can use my dust shoe to extract chips. It works pretty well.
Thanks for your input for the last 2 days I have been stewing over the idea of getting a dewalt 611 to get me thru the aluminum plate cutting. I was not looking forward to the noise but i guess it might be worth doing..I can all ways swap 500w back for plastic cutting. All the reply's help thanks.
I cut plastic too! Acrylic & polycarbonate - I cut way more of those than I do aluminum. Also with the Dewalt & with the same bit, just in 3/16" diameter instead of 1/8". I cut nearly everything I do with these two: Amana Tool HSS1621 HSS Spiral Aluminum Cutting Single Flute Up-Cut 3/16 D x 5/8 CH x 1/4 SHK 2-7/8 Inch Long Router Bit Amana Tool HSS1620 HSS Spiral Aluminum Cutting Single Flute Up-Cut 1/8 D x 3/8 CH x 1/4 SHK 2-5/8 Inch Long Router Bit & I've never used a spindle & I can't comment on the noise vs. the Dewalt, but the noise from cutting is louder than the Dewalt anyway so it's not an issue for me.
Ah geez good point on the noise! Ok im gonna get one. I need the horse power anyway. I haven't cut poly carb yet but i been engraving and cutting painted acrylic. For my simulator I want to build. Cool thx
Sorry Brrian to double reply to same post got some more questions. So ended up with the Makita RT0701 router and you are right the noise for this router at least is close too if not the same as the little 500w spindle and its 1-1/4 hp. Nice!! 3D printing the 71mm to 65mm insert now. Gonna finish my last cut with the last motor end plate. Then move on to my MGN12H Z plate retro fit. I do wonder whats the finish like on the single flute bits us have used when you have cut aluminum? And curious if you have any experience with reducers for the 1/4 in collet? I have some 2mm and 1.5mm bits that need the 3.175 shank. I think I am gonna try this one. https://www.amazon.com/Amana-Tool-P...d=1592763540&sprefix=router+co,aps,218&sr=8-2 I guess if the reducers don't work ill just swap spindles. Those small bits work good with the 500w anyways but just for the sake of constantly swapping. Thanks!
Best makita collet first 1/8 and any other size is probably elairecorp.com/site/makitaroutercollets.html?imz_st not cheap and shipping hurts too cheers Gary
I bought both sets of the Elaire. They are awesome and the metric opens you up to all kinds of endmill possibilities plus the bigger (8mm) endmills for clearing pockets faster. I was using some 2mm endmills on a 4mm shank last night and it was a thing of beauty. Here is the makita link. Elaire Corporation for some reason the one Gary posted was not showing up right for me.
The finish I get with a single flute bit is as good as good as you'd get on any bit as long as you're cutting with the right settings. I usually cut at 40IPM, 21000RPM, .025" DOC. This weekend I adaptive milled some pockets at the same feed & rpm but at .125" DOC; i gave up a little bit of finish quality but a finish pass took care of most of that. And my parts will get powder coated & that will cover whatever's left. & I agree with everybody on the Elaire collets. I have 1/8", 2mm and 4mm collets that I use occasionally.
Ok I appreciate all the advise! I have drawn my own Z plate with linear rails. The motor plate didn't go to good on the cut out with the Makita I realized I might not have had enough feed in to the part I was taking. SO this numbers are good thanks! I keep rereading all the other post and I think its starting to sink in. The other problem I was having with all this info is since I have a 3d printer I've been condition to build stuff in metric. So all the terms in imperial I'm a little slow on. So I found this converter to convert the IPM to MM/Min know I have a reference. I thought it might be useful for others just in case. http://conversion.org/speed/inches-per-minute/millimetre-per-minute I have some benchmarking to do with my machine. So is it common practice if the company that you bought a end mill from produces and speed and feeds calculator would it be good to try to follow there calculator advise for there bit? I also have a small speed and feeds from free trial from G Wizard from CNC Cookbook. But to much info there and I kind of feel like every bit might be built to a specific spec from the manufacture of the bit. Rob Taylor! I had a crash with my 1/4in end mill. Actually I think it was running to slow started melting to much aluminum on the bit and started missing step and z axis plunged into the part. This has happened a couple of times. Well every crash I have, I had to take z axis apart redo all the wheels cause the force of the racking of the stuck bit moved stuff around. Are you talking about the wheels not being sturdy enough or you also talking about whole package and the build of the machine? Like corner plates and holding it together and maybe c beam extrusion themselves do some micro twisting and flexing under stress? So far my wheels have been the first to go in a crash. I know I am asking a lot of this machine!
That's what happens when you're not cutting a proper chip with sufficient evacuation- you have to cut actual chunks of metal, and then get them out of the cutting area as fast as possible! Aluminum is notorious for it. If your feed was too slow or your speed was too high, you were getting too much thinning or rubbing. Lack of heat dissipation is death for tooling. All of the above. Machining metal requires a lot of force and it's not very forgiving. They can do some basic work as plate-makers, but as a dedicated aluminum machine they're not gonna (ahem) cut it. There's a reason a DATRON costs the same as a Speedio (~$100,000), though at first glance it looks to have more in common with a WorkBee. A flute cutting though material at a certain chip size requires some amount of force. The smaller your tool, the less torque it puts on the machine frame to achieve that same amount of force (simple leverage). A tool requires a certain size of chip simply to function- for 1/4", that's about 0.002" (~0.08mm) per tooth. If your machine can't handle the stress that puts on the frame, you can't reduce the size of the chip, because the chip is what's carrying away the friction heat of cutting. You have to reduce the size of the tool, and feed at a slower rate. In order to cut non-trivial materials (some woods and plastics are included in this) you have to understand both the mechanics of the machine itself and the mechanics of the cut and shearing off material. Trial and error is gonna be painful (and possibly expensive).
Checkout the ZrN coated Sharkbits they work wonders to prevent that welding on of aluminum. CNC Router Bits - OpenBuilds Part Store
A "bit" embarrassing (after the post above) but also a milestone for me, I was able to slot cut yesterday! Using a 3mm O-flute, 500mm/min, 0.5mm DOC, 5 deg ramp, Climb cut direction, and a 3 on the makita router (~17000rpm). Babysat the whole cut with air blast and occasional cutting oil, but turned out nice. Should have done a finish pass, but forgot. Not bad for a belt drive Ox machine! Will be getting one of those air/mist kits soon so I wont have to watch it so much. Project is for a strip/disk sander made from an 45 year old bench grinder. Cheers Gary
Nice! FYI I'd use my dust shoe on that - instead of air blast, vacuum takes the chips away. I don't really have a choice... I can't have chips everywhere. But in my experience, vacuum has been enough to clear chips. I'm sure an air blast is better & if the mess isn't an issue for you, no reason to change. & I rarely use cutting oil but if I come up with a way to incorporate something into my dust shoe to deliver it, I'd probably use it more often.
Totally agree, I just ordered the ubiquitous mist/air setup on amazon, hoping to incorporate it into my dust shoe, my vac isn't strong enough to get the chips out of the slot. Part of the success is due to the recent addition of a "quiet" air-compressor (Fortress-2 gallon) from harbor freight, I really like it. Oh and a side note, my machine is in my basement, and when in use my wife and kids typically don't notice it (the noise), except when cutting aluminum! Gary
It did do a nice job cutting that! I was curious of using the oil to cut though does it make a mess of the spoil board. I have not use any cutting oil maybe this could be part of my problem in the long cuts!
I found out the hard way not to have the air compressor for the mister on the same circuit as the CNC and vacuum. Although my breaker was only 15 amps. A 20 probably would have been fine.
I didn’t use a ton of oil just started with a small squirt and another about half way through. The air blasting blowing most of it away anyway. As far as I can tell oil doesn’t make MDF swell like water does so not to bad, the chips still vacuum up fine afterwards. Wd40 is a great option for aluminum cutting too. Cheers Gary
Well I bought some Elairecorps collets the metric pack for now. Price is up there. I probably wont get rid of the 500w spindle as it seems to work on everything just a little slower. I'll Keep it for the smaller endmills stuff. To have all the ER11 collets kind of make you spoiled. Biggest thing now is dialing the use of the Makita. Current i have just put my Z axis back together using the linear bearing rails MGN-12H. Last cut I did was on the mini v wheels on hand drilled plate the proved to work but for aluminum I was finding I was readjusting and re tightening the wheels all the time after every part. And I would have these weird unexplained crashes that would that I think might have been caused by the spindle vibrating or bouncing. Here's a few pics thought I would share the evolution of the machine. With this setup I was able to cut the holes on this plate but i still couldn't cut the part out. I cut bored and made holes in this plate. Now this is the setup to stop the flexing or vibrating of the spindle. Plus the Makita felt to heavy for the other plate and one spindle mount. Thanks for advise! Oh alittle scotch bright almost makes it look like i know what i doing.
