Cutting Aluminum? --- Anyone???

[sharkcutup]

Cut my first aluminum today --- dang clamp got in the way!!! Project was salvageable and as for the clamp; Well it has its battle scars (nasty appearance) but can still do and maintain its job!!!

Have a GREAT DAY EVERYONE!!!

Be SAFE around those AWESOME machines!!!

Sharkcutup

[MDHunt]

Cut my first aluminum today --- dang clamp got in the way!!! Project was salvageable and as for the clamp; Well it has its battle scars (nasty appearance) but can still do and maintain its job!!!

Have a GREAT DAY EVERYONE!!!

Be SAFE around those AWESOME machines!!!

Sharkcutup

I have a couple of questions for you. First, did you practice the design on wood or something else before you cut the aluminum? Also, what bit(s) did you use and what was the project?
Thanks,
MD

[sharkcutup]

I have a couple of questions for you. First, did you practice the design on wood or something else before you cut the aluminum? Also, what bit(s) did you use and what was the project?
Thanks,
MD

My original post was a punn - I was not actually attempting to cut aluminum but maybe one day I'll give it a go. I did not allow clearance for one of my aluminum clamps in my project and accidentally cut into it during a wood carving project (convertible chair/step stool). The project was near completion and I was using a .25 end mill for the profile cutout and ran into the above mentioned clamp.

Have a Nice Day!!!

Be Safe Around those AWESOME Machines!!!

Sharkcutup

[gordread]

Yes, most of my clamps have some battle damage as well. Been at it for 6 years now with my original HD, and still have the original clamps, just customized is all. lol

[Rando]

I cut aluminum on my Shark HD2+ (Rockler Anniversary Edition) nearly every single day. If you have questions and want to learn more, please feel free to contact me. It's not only possible, but done right it comes out fully excellent, if a lot slower than a "real" machine.

That said, yeah, I have a couple clamps with dings. . But, I have far more bits that demonstrate the "height of my learning curve" over the last year and a half . Check it out:

Been bad to my bits for too long....

If you DO want to cut aluminum, the biggest piece of advice I can give is this: investigate "radiused endmills" that have the sharp tips on normal flat-bottomed endmills rounded off via precision grinding. Those rounded corners are far stronger than the tiny tips.

Here's a sample of some simple mounting brackets/assemblies I made. The bracket parts were cut out of 1.5 x 3 rectangular aluminum bar....lots and lots of metal removal .

Cheers!

Thom

[cjablonski]

Wow. Exactly the post i was looking for! Soon I will need to cut a .375 thick block of aluminum 3"x3" to add radius inside corners to it. Of anyone could share thier experience with bits, feeds and speeds it would be extremely appreciated!

[Rando]

Heck yeah....I'll even go one better (assuming this silly system will accept my PDF file).....

Alum6061CutCatalog-Jan2017.pdf

Aluminum Cut Catalog

(651.71 KiB) Downloaded 728 times

This PDF file is my "cut catalog" for aluminum. These are cut parameters that I've successfully used, with the bits indicated, in aluminum, on my CNC Shark HD. Many actual machinists will tell you these are very conservative, very light cuts. And they're right...when bits cost upwards of $50 each, breaking them is to be avoided. Also, I tend to use the same cutting parameters for both flat (pointy-tip) and radiused (awesome!) endmills. If there's anything that's confusing, please do let me know.

Cuts in metal are generally classified as to the resulting surface-finish quality. So, think about making "light roughing" and "finishing" and "fine finishing" cuts. Technically, each cut style represents an overlapping range of step-over percentages. However, no, our machines cannot handle true "rough" or "hard roughing" cuts of much significant depth, so just don't try, okay? Actual, at-depth full slotting is a special and difficult beast that is possible, but risky. That's why there are the several columns in the middle. You'll notice that the harder roughing cuts typically have no information. I'm no fool . Another note, you'll notice that some cuts use the same spindle RPM. This is so I can later combine a variety of toolpaths that use the same bit and spindle speed, and the different cut qualities are created using different proper feedrates.

Another thing you'll notice in the cut catalog is that nearly all my bits are 2-flute. The official explanation is that the chipload needed by the bits, (thousandths of an inch of metal cut per each cutting edge on each revolution, typically 0.0005" to 0.002"/rev), coupled with the available spindle speeds and how fast the machine can accurately move, you're not going to be able to get a very tall OR deep cut with a 4-flute. I'll use a 4-flute finisher sometimes, but only for a very thin finishing pass on fully-flat faces, removing say, 0.002" to create a near-mirror surface. But, if the bit that did the cut right before the finish needs to be done is of the right size and decent sharpness, I'll just use that same 2-flute for the finishing pass, run with the same spindle speed but different feedrates. Honestly, I typically get better finishes with a good sharp 2-flute.

One VERY important thing to remember about Sharks in general is that they don't have bones...they have cartilage. Which means they aren't "stiff". And just like the biological sharks, our CNC Sharks are the same: they are NOT rigid enough to handle all cuts "properly". For instance, you'll find to NEVER use a standard pointy-tip (flat, fish-tail, etc.) endmill in a "push" cut along the t-slot direction. In MANY instances, the tips of the bit pull down the Z-axis ganty (again, because it's made out of plastic, not steel/iron) into the material, and totally ruin the cut. So, I make sure to never push a full-slot cut; only pull, or go along the width of the gantry. You'll learn this the hard way .

A few things I've added to my machine to enable reliable aluminum cutting:

1) A chip blower. A STRONG one. You could use some Loc-Line parts and nozzles and the exhuast part of a shop, vac. I went with one of these as the base blower, bit it's LOUD, so I have it away in the garage. (https://www.griotsgarage.com/product/ai ... rom=Search)

2) A mister. I got along without it for a long time, and mine is not a simple setup, but it has vastly improved the reliability of harder cuts. I use the KoolMist diluted liquid, with a standard mister nozzle from ebay (http://www.ebay.com/sch/i.html?_from=R4 ... r&_sacat=0). I used to use a little timer module to produce pulses 0.29s, every 4.5s. That is a good combination, assuming that just a tiny spritz is put out. Someday I'll post up here information about the mister system, since it's a little "unusual".

3) A machining vise. Okay, I actually added TWO . My fave is the KURT D688 (http://www.mscdirect.com/product/details/09215112), but I also got a "stationary-jaw" vise from MSC (http://www.mscdirect.com/product/details/84397397). I put down three .75" thick aluminum bars under that vise, going full-width across the bed. When those are sufficiently tied down, the bed is FLAT!, which is important, because those vises are HEAVY. The KURT alone is like 25#. If you go with any vise, make sure you can get the bottom of the Z-axis carriage over both the vise and the part. If not, you're going to be limited, and machine crashes will eventually happen. So, you will likely move the gantry up to the top bolt-hole positions to get over that.

4) Deflection is your enemy. That includes both the aforementioned z-axis flex and dive, but also just in the bits. Driving a long bit too hard will snap it faster than you can stop the spindle . That means that, in all cases, use the shortest and biggest bit you can make work. The "best" for this are the "stub" length bits. A 1/4" bit will have like "3D" or 3/4" flute length, and be intended for the work to be pretty close to the spindle chuck. That will improve your cut quality a lot, especially if you're using a router.

5) Cut Feeds & Speeds calculator. I use the CNCCookbook G-Wizard, and LOVE it. Every set of parameters in that cut catalog at one point or another came out their calculator. I can't say enough good about that product.

6) Tramming . If you're going to get into "making parts", real, dimensionally accurate parts, you're going to need to make sure the spindle is perfectly aligned vertical to the bed, and the X and Y and Z of the vise are EXACTLY aligned. As in, ZERO measurable offset. Getting that right isn't easy, but at least it takes a while . It's beyond the scope of this, and you can get by for the first several projects. It's when you start watching carefully, and noticing odd lines on your parts that come from the trailing edge of the bit, and when cuts fail, that's when you'll let out "The Big Sigh" and start measuring and dealing. The good news is you'll start using and loving calipers, setup blocks, dial indicators, alignment squares, machinist parallels, and a whole host of truly gorgeous precision equipment .

7) Tragedy and Terribleness: In Aluminum, SFM or "surface feet per minute" should be your absolute primary requirement. (bit diameter * 2 * pi * RPM) 1000 to 1200 feet per minute for 6061 is optimum for CARBIDE bits (note that HSS bits want slower!). What that means for you is that if you somehow go too slowly OR too fast and the effective SFM is outside that range, horrible terrible things will often happen. If the bit's moving through the material too slowly, it will rub and melt and weld itself to your bit. If it's moving too fast, it will be cutting too much material, which puts too much heat into the cut, which melts the aluminum and welds it to your bit. Noticing a trend here? Yup, either too fast OR too slow can cause calamity. So, calculate correctly, and NEVER use that feedrate slider on the control panel, since it doesn't slow down the spindle rotation, just the movement through the material. The CNCCookbook site has a lot of information about cutting speeds and how that affects the cut.

All that said, be patient. It can be difficult to start, but it is possible, and WAY COOL.

Regards,

Thom

[sharkcutup]

WELCOME BACK - RANDO!!!

WOW! RANDO!

Interesting information, Thank you for your post! I am sure all the Shark enthusiasts here will enjoy your insight and useful information!

Sharkcutup

[cjablonski]

That is, hands down, the BEST informational post I have read in 4 years. It has quelled my concern about an upcoming project requiring machining with the shark. Even beyond that has me kinda pumped to get to it. Honestly, this SHOULD become a thread headed up by Rando to which I would absolutely follow. Awesome info Rando! Thank you!

[Rando]

You're BOTH very welcome!; I'm glad the information is useful to any and all.

You're totally spot-on WRT being excited. I had that too, but when I failed miserably, I just refused to give in to the frustration. It took me a good amount of very careful work making it work reliably (and sometimes daily trips to SwiftTool...see below), to the extent I don't feel nervous cutting metal at all any more. Early on, the bits I chose and the cuts I tried were so far INSIDE what a **real** machine could do, but so horribly OUTSIDE what ours could do, it made me take a BIG step back to truly understand what was going on and how to do it successfully. Little by little....

TEASER:

This is what you have to look forward to....

I want to be really clear on one thing: I am NOT an actual machinist. Not by training, not by profession, and only a fool would hire me for that work. No, wait...only a really smart person would hire me! Yeah, that's the ticket.... Instead, I've learned a lot over the last couple years by doing this pretty constantly, putting in those 10,000 hours. And so, I have to give credit where due:

[*]SwiftTool (and SwitftCarb), in Kent, WA. I'm local to them. They grind their own endmills...high-end and custom stuff for mostly Boeing and their local suppliers. The lines of tools they make go down into the normal stuff we use for smaller work, but not the really small stuff. 1/8" is typically their bottom-end. They are (in my experience, limited as it is) really high quality, and they make 'em in weird sizes (like 2.5" extended-length 3/16" bits...need a small hole WAY down inside something?). You can even have them radius the tips to whatever radius you want (for a price, of course). I could not have been successful without their willingness to look at the issues I was seeing, and in good spirit (as in not flipping sh!t because I don't have multiple million-dollar, rock-solid machines like their other customers) provide their expert guidance. Sadly, their web site is atrocious; I'm not even sure you CAN buy stuff from them on it. Dan and Tarik were stellar in their help. If you give them a call (800-562-0900) they'll send out a printed catalog of their tools. Talk about old-school! Yeah, MSC Direct and other online places are cheap, but having hundreds of years of expertise right next to what amounts to a retail store for endmills? 20 minutes from my house? WITH 5-piece volume discounts and customization? Oh heck yeah!

[*]CNCCookbook.com. Seriously. Even if you don't use their calculators, read their material on machining aluminum. It's clear, reasonably well-written, and gives excellent background to understand what's going on. The more you read, the more you'll know. The guy who runs the site can be an ornery bast*rd I'd sooner stick a shiv into, but the information is good...and I'm a little that way too .

I left this part out originally, but I'll put it in now:

Machining aluminum on a CNC is a little like balancing on the edge of a razor blade. At first, and for what seems the longest time, you fall off every time, or worse, you get cut! It can't be done, you scream. Eventually, you wear the proper shoes*, you find some balance, and then you can eventually stay up on that edge. As you become more and more familiar with that edge, you learn that if you're careful, you can actually move around on it...and next thing you know, you're moving to different areas just to check out the view. The combined Aluminum cutting parameters (depth of cut, stepover, spindle speed, feedrate, tool and material characteristics) ARE that razor blade edge. Yes, almost literally. Compared to wood, the sweetspot for Al is very small (it's even smaller for acrylic!). Once you figure out how to get into that sweetspot, you'll start moving your cutting parameters inside it, and THAT's when you'll really start to enjoy doing the metals. Because you'll start a cut, cringe just a little as you walk away, but when it finishes, you'll come back to this pristine, PERFECT part that wood simply cannot match.

Okay, so here's a GOAL to work for as you start to cut Aluminum. Besides breaking the bit outright, welding melted aluminum onto a carbide bit...well, it ruins the bit, let's just leave it at that . Next down the list of terrible things is a slow condition known as "edge buildup" where the aluminum slowly rubs off onto the bit. You'll see a distinct difference to the shiny parts when this happens. It doesn't ruin or break, but it does dull the edge, overheats the carbide (though for us not usually enough to affect hardness) and at the core, means you're close-but-not-there-yet on the SFM. When you really truly have it dialed in (1050-1100 SFM is da bomb!), you can sometimes cut for DAYS using the same bit and not see any edge build-up and no dulling. Seriously...I ran one 3/16 stub endmill for an entire MONTH until I ran it into the vise . That's your ultimate goal, after all: to cut and cut and cut, and not have to replace those bits for a good long time! It means conservative cuts, but it doesn't mean wimpy cuts. Indeed, edge buildup is often caused by cutting too LITTLE in the pass. I've found its a good, simple indicator of how well my toolpath was built. So, keep that in mind as you progress. Trust me, the day you pull the bit out of the spindle/router after a hard hour-long cut session, and look at it under a loupe, and see no signs of wear at all, you'll smile. Bigly .

I suppose it wouldn't be difficult to just start a new thread/topic. And yet, the topic title is actually perfect. Do we ALWAYS have to make things so darned easy for everyone to find? Maybe it's not always a bad thing to hide useful information behind a good humorous quip. .

Cheers!

Thom

* Okay, no, I'm not saying you **literally** need different shoes to machine aluminum