I watch lots of videos of cutting AL without coolant. Is it reallty necessary?

[rodjava]

Like the title says,
I've watch many videos of cnc routers cutting AL without any type of coolant. Wood routers and high end spindles were used and the cuts appear to be just fine with out using any type of mist, air or flood coolant.

In many of the videos, they were cutting at speeds of 20ipm and faster with single and double fluted carbide bits ranging from 1/4 to approximately 1/2 diameter.

Am I missing something obvious which makes me think using coolant is optional?

Thanks in advance,

Rod
San Francisco

[ger21]

Generally the harder the aluminum, the less likely you'll need coolant. 6061-T6 cuts very well dry. I've had good luck cutting mic 6 cast plate dry as well.
Also, using bits that are designed for cutting aluminum can also help.

20ipm is really, slow, imo. If your machine is fairly rigid, you should be able to cut at 80-100ipm with no problems, provided you take shallow cuts.

[rodjava]

Thanks Gerry,
I really meant to say "as slow as 20ipm"...........

I guess the mister I just bought was for not and a shot of wd40 now and then would have been enough.

I can always transfer the mister to the lathe.

Thanks for making it clear.

Rod

[JerryBurks]

I cut a bunch of aluminum pieces lately (6061, 2011 and 2024 alloys) with 1/4" and 1/8" bits on a very flexible wood router. Had to go quite shallow (0.015 depth) and slow (down to 15-35 ipm depending on overlap) to avoid chattering or stalling my 0.8kW Chinese spindle. But it came out quite well with speeds of 20-24,000 rpm.

The bits made all the difference. I used 3-flute aluminum "S-Carb" end mills from SGS. They cut clean and quiet. I also tried carbide "fishtail" end mills for wood. They clogged up in no time and made a hell of a noisy racket.

I experimented with ispropyl alcohol drip cooling but found it was not needed and actually made the chips lump together while they go into the dust extractor when dry.

[jsheerin]

I always cut aluminum dry on my router. The one problem I have is drilling holes / pocketing really small diameter holes that are close to the diameter of the bit. If I don't shoot some WD40 in the hole, I'll frequently clog the flutes of the bit and break then break the bit. With the WD40 it works great. That probably wouldn't be as much of an issue if I was using the correct rpm for the feedrates I can run, but my router only goes down to 10k rpm.

[ssutton]

Jerry,
Can you tell us where you purchased those 3-flute aluminum "S-Carb" end mills from SGS?

Thanks,
Scott

[hub]

Originally Posted by JerryBurks I cut a bunch of aluminum pieces lately (6061, 2011 and 2024 alloys) with 1/4" and 1/8" bits on a very flexible wood router. Had to go quite shallow (0.015 depth) and slow (down to 15-35 ipm depending on overlap) to avoid chattering or stalling my 0.8kW Chinese spindle. But it came out quite well with speeds of 20-24,000 rpm. The bits made all the difference. I used 3-flute aluminum "S-Carb" end mills from SGS. They cut clean and quiet. I also tried carbide "fishtail" end mills for wood. They clogged up in no time and made a hell of a noisy racket. I experimented with ispropyl alcohol drip cooling but found it was not needed and actually made the chips lump together while they go into the dust extractor when dry.

15-35 ipm at 20-24,000RPM?!!?

[ger21]

I cut aluminum at about 80ipm and 12,000 rpm, and drill at 5000 rpm. I've drilled hundreds of holes in mic-6 dry with no problems. I peck drill at about .05"/peck.

[JerryBurks]

Originally Posted by ssutton Jerry, Can you tell us where you purchased those 3-flute aluminum "S-Carb" end mills from SGS? Thanks, Scott

From MSC . But when I bought them they had them in their "Metalworking Deals" sale catalog for about half the regular price.

[JerryBurks]

Originally Posted by hub 15-35 ipm at 20-24,000RPM?!!?

Well, I know this is a bit unconventional and while these cutters allow for such high rpms (the 1/8" actually even higher), the feed rate should be 100-150 ipm.

But the CNC machine I am currently using does not have the power or the rigidity to do such a high feed rate. And (at least with the harder alloys) these special aluminum end mills do just fine at much lower rates. The job takes obviously forever and it makes very fine chips but the resulting accuracy is good and the surface smooth and shiny. For my one-off jobs I am satisfied.

I suppose the low feed rate takes a toll on the service life of the bits but so far I have been cutting a bunch of parts and they are still good.

[louieatienza]

I pocket at abut 72ipm, and about 12-13Krpm at .125" doc, and halve the doc when profiling. I always use lubricant; you only need a light mist of WD-40 here and there. You will wear you bits out faster without it, in fact almost all manufacturers recommend it. You'll also get a better surface finish.

There are some demo videos on commercial VMCs that do not use coolant; most of these are for filming purposes. Every machining video I've seen where close tolerance work is being done, requiring good surface finish, is done with lubricant/coolant.

I would recommend the largest doc that your machine could handle (and your's is more than capable of it.) You'll get better cuts, less wear on your tools. You want to create chips that extract heat away from the cutting edge; the chips should be hot to the touch flying off the bit. I use dust extraction to get the chips away from the cutting edge, as they will cause problems.

I also would recommend 2-flute bits for most work; 3-flute bits are intended more for finishing work. Also a 2-flute bit would "clog" less. I also use SGS S-Carb bits, but also have used bits from Kodiak Cutting Tools, Onsrud, and Amana. In fact I try to use Onsrud single-"O"-flute bits for most rough profiling.

Here's an example video. I actually had an old can of Cabot Lubri-Tasgon, and it works great as a cutting fluid. I helix in about 4 degrees at .5 feedrate (about 36 ipm). The center hole is actually done at full depth (.26"). The small pockets are done at .1" doc, with a finish pass at .005" doc; and the through pockets at .125" doc. I use a small radial doc (about .025"-.035") so that I can take advantage of using more of the edge of the tool rather than the bottom. When the feedrate and spindle speed are just about right, you get a nice surface finish... BTW this is done with a cheap 2-sided double flute ATRAX carbide bit from ENCO:

DIY CNC Router, cutting BMX chain sprocket, Part 1: Pocketing - YouTube

DIY CNC Router, cutting BMX chain sprocket, Part 1: Pocketing - YouTube

[prcdslnc13]

what cam package are you using Louie? Those tool paths are really interesting. are you doing it as seperate pockets to get the spirals into the star points?