SO3 6061 Aluminum Cut fail

(Dang) #1

First time cutting aluminum on my shapeoko3. It came out gummy at the end.

I thought the beginning part of the cut was okay…

Then the finishing came out to be:

Then I looked at my end mill:

Here is a video of it roughing:
https://www.youtube.com/watch?v=OqOsBoA5rK0

Started with this setting:

My cut started vibrating so I restarted on the same cut with a less aggressive setting:

Not sure what happened but my end mill started gumming up (I think during the finishing). My aluminum plate 5/16" got really hot and melted my 3D printed mounts.

Maybe I ended up with an okay rough but too aggressive on the finish pass? The finish is ugly :frowning:

0 Likes

(William Adams) #2

What we have is on the wiki.

http://www.shapeoko.com/wiki/index.php/Materials#Shapeoko_3

1 Like

(Mark Bellon) #3

Welcome to aluminum and aluminum alloy! It’s famous for this.

This looks like you milled long enough that things got hot enough that the stock and end mill entered the gummy zone. Same end mill for roughing and finishing?

Learning the sound and feel of chatter is a good lesson. With practice, one can spot a problem almost instinctively.

The end mill does not appear to have a coating - ZrN or TiB2 are appropriate. Coatings reduce friction and improve end mill wear.

What RPM are you using? What is the HP of the router?

Dry milling Al and Al alloy requires a delicate touch. On low HP machines I often suggest a single flute end mill. This provides more cooling after each cut.

A spray bottom with a good lubricant - a soy based one is nice - will help too.

The feed rate for finishing should be much lower… 400 mm or even less. A good rule of thumb is the finish rate is going to be much lower than a roughing rate - 2X or more is typically. Fine finish rates can be 4X or less than roughing.

mark

P.S.

On machines where the HP and/or RPM are not easily known - and we cannot use math to figure out a safe feed/speed - even experience machinists will use a piece of scrap stock (of the same material to be machined) - and run feeds and speeds experiments.

Looks like you did that… :wink:

The plate look thick enough that you can turn it over and reuse it. The spoiled side has area to machine so experimentation is called for.

2 Likes

(Dang) #4

it is a 1-1/4 hp with 16k-27k rpm. I had it dialed at 3 on the knob. my endmill is gummed up so now I gotta remove it.

I think I need the aluminum only end mill. I gotta try again.

thanks!

0 Likes

#5

Designxtex, i had a similar problem (see attached) using a standard 1/4 in 4 Flute End Mill - worked ok for the first few passes without lubricant, didn’t realize that T6-6061 requires different tools, talked to a few machinists who advised me, if i wish to run without lubricant,

to switch to a 2 Flute End Mill, which worked well, reduced the plunge rate to 3 in/min, also reduced the feed rate a little to 30 in/min and life has been good for rough work, reduce feed even more for finishing work.

Purchased the End Mills from:

http://onlinecarbide.com
2FL SE REG SQ - TiALN: 212500-C3 $9.95 ea

2 Likes

(Mark Bellon) #6

AlTiN and TiAlN (they are not the same; AlTiN is generally better) coatings are not recommended for Al alloy - ZrN and TiB2 are better choices. The Al in the coating “attracts” the Al one is cutting.

Yes, if one has AlTiN or TiAlN coated end mills they can do Al. Be sure not to push the outside of the envelope - the hotter they get the more the Al in the coating becomes a problem, particularly with a finish.

mark

2 Likes

(Mark Bellon) #7

HSS is fine for Al, just have to have the feeds and speeds correct.

By all means, do use a coated end mill (ZrN or TiB2) - it makes things much more forgiving.

Not knowing the RPM makes it hard to predict - up front - a proper feeds and speeds. Experiments are called for.

Stated bias: I tend to use 3 flute TiB2 coated end mills for Al work on small machines. YMMV.

mark

1 Like

(Mark Bellon) #8

What’s the RPM?

When posting a feed and speed, one must provide all the necessary data. :wink:

If one doesn’t know the RPM, the router, router model, and router setting (e.g. “11”, “warp factor 7”, “ludicrous speed”) need to be clearly stated.

The router setting must be understood as approximate since routers are often inexact about the RPM associated with a setting, even router to router.

By-the-by, there are many correct solutions for feeds and speeds for a given machine and stock. Many are equivalent, others will have interesting side effects.

mark

P.S.

Maybe we should see if someone can paint a line on their router and use a stroboscope to get some idea of what the RPMs for a setting is?

1 Like

#9

Sorry about the missing info, the Dewalt 611 was always set at 5.5, i.e. close to max on the set knob - no way of knowing what the spindle speed was, if we trust the manufactures range and extrapolate - best guess, no load could be 26,000 rpm on this reconditioned model?

0 Likes

(Mark Bellon) #10

Thanks @sliso!

Yup, the feeds and speed were too aggressive, particularly for the finish pass.

mark

0 Likes

#11

There are a lot of factors that go into getting a good finish with aluminum. Here are a few tips that have helped me greatly:

1- Cutting Direction: With all non-ferrous metals you want to “climb cut”. That is to say, you want to feed in the same direction of the tool rotation. So when the flute contacts the material it is pulling it instead of pushing it. This is probably the single most important thing you can do to get a good finish but is tough to control using CAM programs that don’t do it automatically!

2- Material & Temper: Not all aluminum is the same. Even within the same grade! Some are good for forming and others better for machining. Grades that form better will machine like hot boogers. The grade you get at the hardware store usually sucks. You need to pay attention to the temper as well. For instance, 6061-“T6” will machine much much better than 6061-“T5”. The T6 temper makes the metal harder and form chips better so cutters are less apt to gum up. Starting with the right material with the right temper makes all the difference.

3- Speeds & Feeds: You want to make sure you are “cutting” and not “pushing” the metal. You want to make a good chip. So if you run your RPMs really high and feed really low you are not taking a cut and just making friction = heat = gummed cutters. If you were to run a spindle at anywhere near 10k RPM you would have to run really high feeds. To do that you need a really rigid machine, which these are not. So going lighter is not always the answer. You might want to try feeding faster and turning the tool slower. If you try to take a fart skin thin pass at high RPM you will just push the metal and swirl it up. The cutter needs to engage in the material. So take a cut.

4- Cutters: Anything considerably harder than the material will cut well. HSS works just fine. I do use uncoated carbide because you can get a little better finish and be a little more aggressive. However, most of this is based off of the rigidity of your machine. Given that most of the machines in this realm are made from aluminum themselves, you can only be so aggressive cutting the same or like materials. You don’t want to get a cutter with any coating that has Al in it. Like materials stick to each other. This also generates friction/heat. At best the coating will just wear off. It is more likely that it will gum up and break tool. Probably when you are almost done with your part. The TiN coating works good (gold in color), but is probably not needed unless you really have a serious CNC machine that is taking heavy cuts.

5- Experience: You will know when you have it right. When you are machining aluminum with the right parameters it sounds really good. It is a very satisfying sound. It also produces a surface finish second to none. I wish all parts could be made from aluminum…

Hope this helps! Good luck!

2 Likes

(Jonathan K) #12

Sean, these are all good suggestions except there are some caveats to #1—roughing vs. finishing, because of chatter and deflection.

This is especially true for those working with the So3 rather than the Nomad, especially earlier So3 kits that don’t have the L-angle bends in the z-axis plate, which means they’re prone to chattering during climb cuts traveling on the y-axis.

For finishing passes (and on the So3 in particular) YMMV on climb-cutting vs. traditional with the belt-driven machines, which is why I hope to upgrade sometime to the Nomad Pro!

1 Like

(Jonathan K) #13

@sliso I’m digging your t-slot bed, and also your reinforcements of the z-plate. Any notes of advice on that?

0 Likes

#14

Union,

True. On a roughing operation it doesn’t matter much what you are doing. You are just looking for a “rough” finish. I also don’t have experience with the Shapeoko so I can’t speak to that specifically.

Generally speaking, it is all about the rigidity of your set-up. From looking at designxtek’s work holding set-up I don’t know if you could ever cut aluminum well there. Specifically, the MDF type material waste board and wood or plastic side clamps will probably never hold the aluminum work piece without chatter. All of those weaker materials are destined to deflect as you apply forces to the relatively stronger work piece. There is also no vertical force holding down the work. If you compare that to sliso’s nice looking set-up, he has an aluminum table and vertically clamping hold downs. That would make a huge difference and I am sure eliminates much of the chatter and would allow for the more taxing climb cuts to be made (at least made easier).

I will add this last tidbit: Use the shortest possible cutter length. If at all possible, use a stub style end mill. Only leave as much shank exposed as you need to reach the depth you need. I realize that many routers don’t give you much throat to stuff the cutter in too deep. Choking up on the bit and leaving as little as possible hanging out of the collet can make a big impact on chatter.

1 Like

(Leith) #15

Looks more like friction stir welding than milling :slight_smile:

2 Likes

(Aroldo de Rienzo) #16

Carefull with overheating.

As many said, aluminum tends to heat up a lot. I havent done this on the nomad, but on the manual ones that I have, a coolant is very efficient. Also the right tool.

There are some that are very effective that have replacable bits in order to save up on complete bits. These are ceramic or carbide and are very good. The best in my opinion are Mistsubishi or Sandvik.

Both give great customer service, you can call them up and tell them the material, you are dry milling and anu other things you see necesary, they’ll ask you some questions and recomend the best cutter. Sandvik even guarantees the amount you can cut one on tool before the bit or the tool breaks.

I was having trouble milling and lathing Hastelloy C-276 (Hardest material ive had to work with), these guys gave me the right tool, RPM and NOTE, when I told hem I was dry milling, they changed the tool and geve me a better one.

http://www.sandvik.coromant.com/en-gb/pages/default.aspx

and in the US:
http://www.sandvik.coromant.com/en-gb/contact/pages/findus.aspx?cc=us&cat=2

hope it helps.

1 Like

(Mark Bellon) #17

The real challenge on the SO3 is we’re not really sure of the RPM. If we accurately know the RPM we can - up front - calculate a safe and effective feeds and speeds. Dry, air cooled or wet we can hit things pretty darned close without an experiment.

ZrN or TiB2 coated end mills really help - they are “slipperier” and generated less friction; last longer.

Al alloy on small machines with dry machining can be done quite nicely with a single flute end mill, specifically designed for this purpose. Here is an excellent article that explains things:

http://blog.cnccookbook.com/2012/12/23/why-use-a-single-flute-end-mill

Want to try a single flute for Al alloy? Onsrud 63-400 series (soft Al), 63-600 series. Nomad? I would recommend the 63-604.

Bias: Onsrud makes AMAZING machine tools. They may look expensive but they are crafted “insanely great” and last a long time. They are worth every penny.

mark

1 Like

(Dang) #18

thanks everyone for the feedback!

I will try my cut again with a lot of adjustments and see the results.

0 Likes

#19

@UnionNine, to answer you questions an perhaps you may be considering similar modifications for similar reasons, I was considering the following;

  1. Need to machine long profiles (approx. 20” in length, in 2 steps) and hold firmly.
    Replacing the waste board with 80/20 extrusions (10 series, using combinations of 1010, 1020 and 1030 extrusions) seemed simple, had been done by others to stiffen up the table and allow multiple holding points, seemed to be a good solution to work with longer profiles (held beneath the table). While the bed is more robust than the MDF waste board, the 1010 extrusions are a little to light in spanning the S3 bed unsupported for my liking, if I was to do it again, I would use the 15 series.

Approx - $180 plus $50 nuts and bolts, made the plates from scrap lying around

  1. Need to machine taller items 3” x 3” angle.
    The 80/20 extrusions also could accommodate larger work pieces as the modular sections could be removed at will. Here we needed to raise the table some in order to access the holding clamps, so 6” legs from 2020 extrusions with leveling pads were installed. This worked very well – please see attached photos

Approx - $30 plus $5 nuts and bolts

  1. Need to minimize some of the tool creep in the z-axis during tight plunge or drilling operations.
    Found the cantilevered configuration of the z-axis allowed the bit to walk no mater what reasonable settings I used. Saw another S3 on one of the forums that used simple stiffener from ½” x ¾” aluminum bar stock. Looked like a good idea, so I copied it also. Still not as stiff as I would like, perhaps ½” x 1” steel angle would have done better, but I cant help feeling that the cantilever design will always have a little play. Perhaps I’m asking too much.

Approx - $6 plus $2 nuts and bolts

All in all, the machine is now doing what I wanted, repeatability is good for this machine, so I’m very happy with the system and the mods to extend the range.

1 Like

(Mark Bellon) #20

I use T-slots myself - 80/20 equivalent - and over the years I’ve pretty much given up using the 10 series stuff. Unless there is a space restriction that requires it, I use the 15 series stuff.

One of my CNC machines had a bed made from 15 series T slots. Used the CNC machine to flatten the top.

mark

1 Like