Aluminum Cutting 101.

Aluminum Cutting 101.
It seems that there is some interest in how to cut aluminum so I thought I would put together some tips and thoughts from my experience since I have been doing it for awhile and since I learned so much from the Laser forum, hopefully I’ll be able to help someone else.
As I share this information keep in mind your experience may differ based on your specific machine. Many variables can affect the outcome of your experience, things such as gantry height, table rigidity, spindle power etc. I use a MultiCam “M” series, 5’x10’ table, with 4hp Colombo spindle and stepper drives. It has a vacuum table and I use MDF as a spoilboard. It was built in 2001 so it’s getting a little long in the tooth but still does a good job for what I need.
There are only two types of aluminum alloy that I use, based mostly on what our shop produces and what is readily available from local suppliers, 5052 and 6061. Breakdown from my supplier.
Aluminum (5052)
Available in sheet. 5052 is the alloy most suited to forming operations, with good workability and higher strength than that of the 1100 or 3003 alloys that are commercially available. 5052 is not heat-treatable, but is stronger than most of the 5xxx series of alloys. It has very good corrosion resistance, and can be easily welded. 5052 is not a good choice for extensive machining operations, as it has only a fair machinability rating.
Aluminum (6061)
Available in Angle, Channel, I-Beam, Pipe, Plate, Rectangle, Round, Sheet, Square, Tube. 6061 Aluminum is, by most any measure, the most commonly used aluminum alloy. It is specified in most any application due to its strength, heat treatability, comparatively easy machining, and weldability. If that were not enough, it is also capable of being anodized, adding a layer of protection for finished parts. The main alloy ingredients of 6061 aluminum are magnesium and silicon.
I use mostly 5052 because it costs less than 6061 and it’s softer and easier to work with for the most part. The only problem I have with 5052 is that the sheets don’t usually lie as flat as 6061 so sometimes it takes some extra fixturing like screwing a corner down.
I always start by masking one side of the sheet with some paper pre mask. This serves two purposes, first it lets me cut to the paper instead of into the table surface, second, it helps to hold shapes in place and maintain vacuum strength while cutting.
I use a misting system on my machine, specifically the Trico MD 1200 dual mister. It’s a bit more expensive than most misters but when it’s properly dialed in I can run my machine for 8hrs strait and not have to refill. I use it with their synthetic lubricant http://www.tricocorp.com/products/product.aspx?c=5&p=60
It goes on very fine, doesn’t make a big mess and is easy to clean up, also I have had some bits last well over 100hr lifespan before they start to dull out, at $30-$40 per bit, that adds up. Scott Shepherd told me he was having problems using coolant which I assume was going on too heavy and because it’s a water based coolant it was soaking into his spoilboard and causing damage. With the synthetic lubricant I am able to avoid that problem.
There seems to be two basic applications, cooling and lubricating depending on the type of material you are cutting. With certain dispensers and fluids doing a combination of both, ie. certain coolants have some lubricating abilities and some lubricants have cooling abilities. This article explains better if you're interested.
http://www.tricocorp.com/pdf-files/micro-dispensing.pdf I notice that some people don’t use any lubrication but instead do a dry cut, more power to ya if you can get away with it but I notice that they are doing it in many shallow passes vs. one or two passes. The problem I have with this method is that unless you get it dialed in just perfect you will experience “re-weld” of the aluminum onto the bit which will dull your bit faster and leave a nasty burr on the edge of your material. Remember you are creating heat by the friction of the cutting process, so it makes sense to me to use a lubricant with cooling properties so you avoid that completely, especially with the softer alloys. As a general rule I always use the formula of 1 pass x the diameter of the bit, ie. If I’m cutting .25” aluminum with a .125” bit I will do it in two passes, .125” aluminum with .125” bit in one pass, etc. This is where the different machines may vary in their ability. You may want to start more conservative and take an extra pass, you need to find what works best for your machine. The nice thing about cutting .25” aluminum with .25” bit in one or two passes is the size of the waste that is produced is much easier to handle, ie. Big chips are easier to clean up than splinters that get into your clothes and under your skin.
I prefer to use the Onsrud 0 flute 63-600 series cutters mostly because I can get a good price on them. I’ve used Belin as well and they are at least equal in quality IMHO. Double fluted End Mills will work fine for the most part too, if that’s what you have available, use it, but when you have piles of shavings to clean up you will appreciate the single flute bits.
Speed and feed rates tend vary widely in opinion as well. The bit manufacturers and the machine manufacturers will usually tell you that you can cut at very high feed rates which is possible in the short term but not always practical in the long term. Again this is where testing and trial and error on your particular machine will need to be done. Here is a link to some speed and feed rate charts from Onsrud that will give you a base line to start from.
http://www.onsrud.com/xdoc/ChipAluminum
Again these tend to be on the high side in my experience but I tend to be more conservative because when I first started using this machine I was too aggressive and ended up having to replace spindle bearings within my first year, I had to back-off a bit base on what my machine could handle, I’m sure a heavier duty machine could probably go faster. I will sometimes adjust my settings based on my production schedule. If I have a big job that will take days of routing I will bump up my speeds but if I’m not under too much pressure I try to run more conservative in order to cause less problems. My conservative settings and where I would feel safe starting an unknown machine at are; 3/16” bit, ¼” aluminum sheet 5052, 2 passes, 15000rpm, Z plunge-6ipm, feed rate30ipm. Adjust up according to what your machine works best at. For high production I think somewhere between these settings and the Onsrud formula is probably more realistic. Listen to your machine, as you get used to it you can tell by the noises it makes as to what’s normal and what’s not. If your machine starts to sound too loud and scary, back it off some until it sounds better or add an extra pass. If the aluminum is sticking to your bit, that is melt-back, your bit is melting the aluminum and you are creating too much heat. First make sure you are getting proper lubrication, then cut back your speeds until you stop seeing the melt-back.
Fixturing small parts or letters can be tricky sometimes when part or centers of some 2” tall letters start flying across the shop or binding up and snapping your brand new ¼” solid carbide bit. To deal with this I usually try to use “tabs” when I set-up my tool paths. I use Enroute 3 pro but I think any decent tool pathing software should include this feature. You can usually get away a pretty shallow tab, about .02-.04” thick and about .125”-.25” wide. I try to get away with as few as possible, maybe 3-4 per part. If I’m cutting out of a smaller scrap, I will often use a good double sided tape to help fixture as well.
There are also many helpful resources on the Onsrud website concerning CNC cutting, worth a look if you if you’ve never seen it. http://www.onsrud.com/xdoc/Resources
Wow, I did not intend to write this much when I started. Some of this may be old news to many of you so hopefully I didn’t come across as a know it all and hopefully people will benefit. If I made some mistakes or if you disagree on a point, please feel free to correct me.
Paul Phillips

i am currently machining a small cover to hide the bolt heads on an aluminum column in a football stadium, joe expert sold me 3003 alu and i got a good lesson in the numbers of aluminum!! the "box" is an 8"x8" with corners notched .7 in order to fold, the center is cut out inside 4" x4" to slip over the post. the next expert sold me 6061 / .1 thick and i got another lesson in how the harder alu breaks when folded!! today i finally have success with 5052 .063 (machines and folds) got a good education in aluminum this week and am glad you are posting here. i found my way into "charleston aluminum" kinda like the disney land of aluminum.

thanks for posting, i for one will be watching

jim

Thanks, Paul. I am building a steel framed CNC router, so I kept a copy for future reference.

John

Paul,

Any useful tips for machining brass? :D

Brass will be a lot easier cutting than the aluminum as far as all that chip welding and such you experience with aluminum. The problem with brass is that it has a tremendous amount of stress in it from the process of manufacturing it. Once you break the skin, where all the stress is concentrated, it bows like a banana. You can reduce it and through proper machining techniques, you can pretty much eliminate it, but just know that brass has a ton of surface stress created as it goes through the rollers to make the size (if we're talking bars, not sheet), so if you need something to be flat, know in advance, you might run into issues. All of them can be overcome, but it's an issue.

Thanks for posting this Paul. Great insight and information.

So for brass bar... lightly machine one side flat, allowing it to bow in the process. Flip it over so the newly machined side is against the table and machine reverse side.

I wish it was that easy :)

There are several techniques, some a little too complicated to describe in words, I'd have to draw something up, but one method is to cut it on all the sides you want, allowing it to bow, and then come back and machine it again, but holding it a free state when cutting it, meaning don't take a bowed piece, clamp the bow out of it, cut it, and then release the clamps. You'll have nicely machined parts, that are parallel, but they won't be flat.

It's commonly done in vises, like a Kurt vise or a series of Kurt vises. They are super square. So you can clamp it, cut it, then once you have a "flat" side, there is an order and direction of which side to cut next. That'll get you flat and square all the way around.

Probably way overkill for what most people would use it for, but if you want it square and flat, it's not as easy and just cutting it and moving on.

I wouldn't worry about it under you have issues that are stopping you from a quality standpoint.

Dan, like Scott said, it depends on what you are trying to cut, billet or sheet.
Scott, it sounds like you are describing more of a precision machining process for a mill. I've never run into the problem you are describing but, I haven't cut much brass, just some letters out of 3/16" and 1/4" sheet and it cut fine. I think you're supposed to reduce the RPMs a bit but I think the settings for aluminum will work pretty good.
Paul

A tip for final pass on aluminum is to CLIMB cut. Finish is so much better. Your setup needs to be solid though because the cutter will try to pull the work toward it. So, Light cut (.005"), normal cutting speed, clear way previous chips and use some cutting fluid. You'll be surprised at the finish you get. This refers to cutting around a shape, or in a pocket with the side of an end mill.

Thanks for posting this and a bump of a great thread.

I'll add two things:
Keep the kerf clear of chips on multiple passes.
Allow for a full doc pass at the end

Use coolant