[dbtayl]

I've got a home-made mill that I'm using to cut some aluminum parts for a project of mine. The part in question you can see here (54mm OD for reference):

https://fc65b08ce27786f4d35a7e557ff4...0140803_00.jpg
https://fc65b08ce27786f4d35a7e557ff4...0140803_01.jpg

I'm cutting these parts from a piece of aluminum bar stock, which means that I need to do some full-diameter cutting to cut the final piece from the bar. My setup:

11250 RPM
1/4" 2-flute carbide end mill
22 IPM feed
0.02" DOC

For the internal pockets you can see, the cut sounds good. I'm spiraling into the cut, then working out to the edges (for the internal pockets); the spiral in seems to have some chatter, but it's not too bad.

For the circular cut to extract the piece from the bar stock, the cut sounds... wrong. I assume it's chatter. In any case, it cuts OK (as you can see from the pictures), but I don't like the sound, as it seems like something is wrong. Even if that's just shortening tool life, I'd like to fix it.

I'm not using any coolant (I don't have a mister or anything) or anything to remove chips (or lubricate) during the cut, so that may be some/a lot/most/all of the problem.

My machine is of no specific design (I built it myself from no plans), but it's a 3-axis mill with one of the 1.5 kW Chinese water-cooled spindles. The axes are leadscrew driven with 176 oz-in steppers, 12 TPI screws, and Gecko drives. I kind of doubt all that's relevant, but the spindle certainly is. This is about the best picture I have, it if helps:

https://910d3b72b50f8f8fe4bb72a001e5...0140322_01.jpg


Suggestions on things to try? My best guess is that I want coolant/lubricant and a higher feed rate (0.002 IPT or more?), but I thought I'd ask people with more experience than I. Adding an actual coolant dispenser to my setup would probably be a pain, since my table is MDF (not to mention the machine being wood), and MDF + oil/water/whatever doesn't seem like it would end well. Maybe just spraying oil on the cut as it goes?

Thanks in advance!




For reference, I should add that I don't have much manual milling experience- just a little bit of incredibly basic stuff on a huge Enco. I've done quite a few hours with a [metal] lathe, though.

[tc26]

From your description of the machine and the picture you posted, I would say the problem is related to the lack of rigidity of your machine.

[diamond.3211]

I agree with tc26, but something to get those chips out of there would definitely help. Coolant when cutting alum. is used as more of a lubricant than as an actual coolant so is not an absolute necessity, but some air directed on there to remove the chips from the cut, even if it is nothing more than an air nozzle and compressor that you use manually would probably be your best bet, with the wood and all.

[dbtayl]

So messing with speeds/feeds/DOC isn't likely to help much?

For improving rigidity, I assume the best bet would be rebuilding the structural elements with metal? It seems pretty rigid to me as-is (though I'm only a hobbyist in the realm of mechanical construction). Or maybe some sort of cross-bracing would help?

With regard to lubricant, I've got thread cutting oil and 3-in-1 handy. I assume either of those would help? I think I've read kerosene is recommended for aluminum lubrication as well.

Thanks!



EDIT: I've also got some 1/8" 2-flute end mills. My impression is that a smaller tool will just exacerbate the chip clearing issue (no?), but any idea if it would help with chatter? It seems like smaller tool -> higher resonant frequency, though that may not be relevant if it's the machine in its entirety vibrating...

[Eldon_Joh]

so the table slides under the fixed gantry?
if that's the case you might simply build a bigger box around the gantry.
is the gantry a box or is it open inside and accessible from the back?
at least make it a closed box.
The sheer force acting on what looks like about 1 foot by 1 foot by 1.5 inch press board (rigitidy in the left right axis, i'll call it X as shown in the photo) are probably the weak axis with regard to rigidity

also depending on how far the spindle is from the box, torsion forces exerted on the gantry also exxazerbate the issue in the X axis

if the gantry isn't a closed box then forces in the Y axis twist the entire box and that also causes the spindle to deflect up or down. if its a closed box i don't see much way to beef it up without completely rebuilding it.

[dbtayl]

Yup, the table moves under the gantry. And now that you point it out, the side-to-side axis is probably less stable than it could be. Here's what the back looks like (or did; the structural elements haven't changed):

https://910d3b72b50f8f8fe4bb72a001e5...table_back.jpg

The spindle is about as close to the axis as I can reasonably get it. I'm not aware of any other design that would reduce it further, though I'm listening if one exists.


I guess that gives me a starting point... I'll play around with feeds/DOC/lubricant and adding structure to see what happens.

Thanks for the suggestions!



As a side note, other pictures and whatnot here:

https://sites.google.com/site/dbtayl/cnc-mill

[Eldon_Joh]

ok, it looks like you can glue a single piece of wood in there to make a three sided box or you can make a 4 sided box.
also, it appears you can screw a sheet of wood or metal to the back and close up the entire box.

[AiR_GuNNeR]

Your feeds seem way low at that RPM. At 6000 RPM, I normally cut at 35-40 in/min. Your DOC is backed off enough to compensate for lack of rigidity. .125" DOC is pretty normal for slotting with a .250" EM. If you don't feed fast enough, your cutter won't bite into the metal, rather tend to rub more. You will also want to use lubricant. When I used to run my X2, I would keep spritzing WD40 while cutting so the cutter didn't load up.
Eric

[dbtayl]

I did some quick testing yesterday with a chunk of scrap. It's probably not the same alloy I have been working with before, but so it goes.

Anyway, feeding at 34 IPM at as much as 15 mil DOC seemed to work just fine, so long as I used some lubricant (I tried generously applying both the aforementioned 3-in-1 and thread cutting oil, and both seemed to work fine). Perhaps more relevantly, the edges of the cut were nice and shiny. My previous attempts ended up having what I assume are chips stuck to them. See edges here:

https://fc65b08ce27786f4d35a7e557ff4...0140803_01.jpg

I haven't tried running faster/deeper yet, but I'm getting to it. I DID clean out the chips every couple passes, and I was doing straight feeds instead of helical, so it's likely not an entirely fair test. Would feeding in both X/Y and Z be likely to cause resonance changes? I feel like the Z feed has been low enough (20 mil per revolution around a 60mm circle) that it's probably not the problem, and more likely chips/rigidity.

In any case, I think things are generally looking up. I was previously running at a 1 mil chip load because I seem to recall reading that was suggested at some point, though that may have been for 1/8" end mills. Now everything I'm reading is saying 2-4 mil or "however fast your machine can handle", so I guess I was a little under.

I'll try to post some more comments when I get to do some more work.

Thanks all!

[AiR_GuNNeR]

Glad it's looking better! It took me a while to trust increasing the chip load. It's just a matter of finding that sweet spot. Early on, I would break a 1/8" end mill so I kept decreasing the feed rate, which made things worse because I was simply rubbing the snot out of the end mill and aluminum. i would have a ridge of metal on the edge of the cut. Calculatge the RPM required to get the SFPM for the material, then calculate the feed to get the recommended chip load. The DOC can then be increased based on your machine rigidity, cooling, etc. Generally, you will want to keep the DOC at a maximum half the diameter of the end mill.