Aluminum

[newton_c]

The bot has been great for our plastic channel letter faces.

But now I am trying to cut .040" sheet aluminum channel letter backs.

I have a 1/4" CED 2 flute, straight bit running at 12,000 RPM's, moving @ 1 IPS, and the Z @ .40 IPS. I use perimeter screws and double sided tape for hold down and it isnt moving or pulling up when cutting.

It is leaving a nasty kinda folded up, very sharp edge on both edges of the cut. Folded straight up at about 90 degress to the sheet and making some nasty snagging type of cut sounds as it moves. I just ran it a foot or so and stopped it.

Any ideas to get me closer? It seems I am a long way off now.

[Brady Watson]

Change the geometry of the bit. Use either a standard 2-flute end mill (like an upcut spiral) or ideally use a single spiral O-flute. The difference will be amazing. Your speeds & RPM are in the ballpark.

-B

[newton_c]

Thanks Brady. I have several new 2 flute end mills (both up and down). It seems to me a down cut would be less likely to lift from my holddown setup. Would a down cut dull faster or something? Is there another reason you recommend the upcut?

I will try this out Monday. Continued Thanks!

[Brady Watson]

Downcut spirals are a little tricky when it comes to AL and plastics. They tend to throw the chips back down again and make the bit run hot. The only downcut that I would try would be an Onsrud Super-O downcut. It's a single spiral-O but downcutting.

Many times climb-milling aluminum results in a better edge quality than a conventional strategy. You might want to try this with your straight as is to see if you get a better cut. Question: How does the scrap material look? Does it look better than the desired part? If so, switch strategies. Try cutting one part using conventional & one with climb when trying out different bits. You'll find that one cuts a lot cleaner than the other, or at the very least, leaves a nicer edge than the other does.

The tape and screws with that thin sheet gets ugly after a while...the screws tend to distort the sheet (even if you can't see it) and the tape residue on the bit just gums everything up and makes it run hotter. Tape on AL is only good some of the time, as the AL heats up, the tape wants to fail. It would be worth looking into making yourself a suitable vacuum fixture, even with just a shopvac, if you are going to cut AL on a regular basis. I use vacuum to hold AL sheet up to 1/8". Above that and I mechanically fasten it with coarse screws. Over 1/8", there is enough meat to the AL to not deflect or dimple, and cause another part of the sheet to pop up.

-B

[john_l]

The heat is the thing to watch, as you suggest.

I did try my same settings with an upcut, 2 flute spiral. I essentially had the exact same results. The edge is heating and tearing rather than cutting. The aluminum is sticking to the bit. The bit was new and I checked.. I am climb cutting but the edge is equally messed up both sides (waste side / part side). I didn't see the sheet move at all and it hasn't passed through any tape that I can see as of yet. I appreciate your input.. I will keep experimenting.

The machine has the power, the spindle isn't even warmong, I think, as you've stated, I just need the right bit to get it done. I will later put together a vac hold down as long as this works well. I just want to see it work on a sheet or two first.

I just realized I have 2 acocunts here.. I am NCheth also.. Cheth is our shop manager. Hope I havent been reponding to my own questions.

THANKS!

[Brady Watson]

John,
You might want to try an air cooling setup, blowing on the bit. On thin sheet metal an o-flute doesn't seem to need it. If using anything else or milling thick AL like 1/4"+ (I've done up to 3/4" on the Bot) compressed air is definately needed to keep things cool. Even with compressed air, things get toasty.

There's some info on it here (http://www.talkshopbot.com/forum/messages/29/22527.html?1184729271) Just build the setup and point it directly at the bit.

-B

[john_l]

Brady... man-oh-man... I just got in from the shop. I found a bit in a drawer from the guy that I bought the bot from (used). It was an Onsrud 1/4" SE UPCUT SPIRAL SUPER 0 FLUTE PN: 65-025....

Wow! Like a hot knife through butter, perfect edge on both sides of the cut, throwing perfect 1/8" - 1/4" curly shavings, just awesome.

This bit was used but didn't have any discloration or anything, I chucked it up and ran the same file I had been trying with the other bits... it started moving...passed beyond the previously cut at areas into some new material... and my jaw just dropped.

This is exactly how I invisioned the bot working for me. This is called "the hookup".

Thanks Very Much.

John

[joe]

JH,

A couple of week ago we sliced throught eleven (4'X10') sheets of .040 with relative ease. I thought I'd share my experience in hopes to give a little insight.

A point of importance is the alloy type. My customer drope shipped ten 4'X10' sheets of 5051 and sliped in a 6061 brushed anodized 5'X11'. We ruined that one strait away. All letters were to be cut out as relief and that gave me indigestion. You just can't make any mistakes. None. More acid indigestion. burp! Why O why do I ever get into these situations.

Onsrud informed us that a coolant would leave colored heat rings. O great! Fortunately we didn't need it anyway.

While our spindle speed was 14000, the feed was double yours. We used, what I believe is the best bits on the marked, Baliyn O up-spirle. There was a very signt razor edge on top but the sides were mirror smooth.

I bridged all copy with a short slow down raster. Also we drilled a very small hole in each corner of the sheet for a screws to keep it in place. I zero'd to the bed, which goes with saying. Anyway.

Let me say again: I'm no expert in this area, however it worked like a dream and I think it's due to the Bailyn bits and Rollaids.

[Brady Watson]

"I think it's due to the Bailyn bits and Rollaids" LOL!!!

Here's a couple shots of 3/8" AL plate that I cut for a motor adapter for my Bridgeport mill last week on my Alpha. The original motors are NEMA42 size and the replacements are NEMA34 size. The original AL pulley for the Z axis was worn out, and nobody makes a repro one in AL...so I had to get a steel one. It weighs nearly 6 pounds! In the pic, you'll see a thrust bearing to take the weight of the pulley so that it doesn't wipe the bearings out of the stepper, just below the 5/8" to 1/2" shaft adapter.

At the moment, this is a PRT 4G powered mill running SB3. Not everything is fully operational yet, but it will be the 1st and probably only ShopBot controlled Bridgeport CNC in the world. I really love the ShopBot interface & wanted to go with it on the mill since I know it so well. Also planned is an Alpha version, which should really get this thing to boogie!
Hooking up to a 4G or Alpha board is a cinch, for those that might be interested in retrofitting an old tool at some point...I'm even considering putting SB3 on my CNC lathes...but that's down the line!

At the moment things are in 'test mode', somewhat greasy and not ready for prime time just yet. Unit values are 10,000 with the G202's microstepping (2000 steps per rev * 5:1 ballscrews)...anyway, here's a couple pics of the mounts done in 3/8" 6061 AL. The plate was drilled, screwed to the table and cut @1.2 IPS with a .0625 step down, 13,000 RPM using a 1/4" HSS end mill & forced air cooling. I found that the HSS really soaked up a lot of vibration and resulted in a smoother cut. The HSS also seemed to be sharper than the carbide end mill I used. The carbide end mill seemed chatter a bit more and like climb milling better than conventional. The opposite was true for the high speed steel bit.

While my Alpha isn't a heavy mill like the Bridgeport, it sure is nice being able to machine components like this rather than having to cut them by hand. Edge quality is pretty darn good for a router


-B



6643

6644

[paco]

Nice work Brady! Smooth cut indeed.

The machining specs. are relatively good considering the 6 foot PRT gantry.

I may order some HSS again to try on AL; so far the one I've tried were not very good in wood products... I haven't tried in plastics... I did heard that HSS was the #1 choice for AL but I was in doubt since a router turn way more faster than a metal mill spindle. HSS doesn't tolerate heat very well. I did heard too that HSS tools are sharper than solid carbide ones.

Thanks for sharing.

[Brady Watson]

Thanks Paco.
I don't like HSS for sheet goods and was a bit leary the 1st time I used HSS for AL. It really does make a difference and they are also much cheaper. I pretty much use nothing but OSG brand carbide & HSS since they are such good quality.

-B

[paco]

Brady (or anybody else),

have you tried HSS with Alupanel/Dibond? I wonder if the cut would be as good and if the cutter would last as long or a bit long... if I could cut down on cutter fee when processing this material, I'd like that!

[Brady Watson]

Paco,
I haven't tried a HSS in Dibond...but it would be worth a test! I have a fresh sheet of the 4mm stuff here...although I don't have any immediate projects to cut out of it. I'll give it a try when I have something that needs to be cut out of it. All of the Vbits I have are carbide. I wonder if a HSS Vbit can be had...I know Amana sells 91° Vbits specifically for cutting dibond so that you can over bend it a little to get your 90° corner.

-B

[john_l]

Thank you Joe (and all). I will look into the Bailyn bits as well.

I cut up the 8th sheet of 19" high channel letter backs with this Onsrud bit I found today. It's still moving through like when I started using it. I haven't noticed any change in the cut, shavings, or sound.

I never thought I'd be asking... How do I know when I have to retire this bit? Will it be as obviously screwed as my earlier attempts?

[Brady Watson]

When it starts 'smearing' like it was before or edge quality degrades beyond your tolerance.

-B

[john_l]

i found the limit of the 1/4" O bit I suppose.

This was 1/8" aluminum that I was cutting as base plates for a roof mounted satellite dish for our motorhome. I managed to get 3 good ones and then the bit started smearing. I attached the file in case anyone would take a look to see if I had anything wrong in the settings.

I had already cut several sheets of .040 aluminum with this same bit and it did fine so I got my moneys worth of the bit. Thanks


6645

[john_l]

File was too large.

[Brady Watson]

John,
A couple things....

1st, you should really used compressed air cooling blowing on the bit while it is cutting to reduce cutting temps. This means taking off the dust foot. The dust foot & dust collector provide some cooling for thin sheet metals, but not enough for thicker materials that tend to get 'heat soaked'. Heat is the killer of bits and metallic parts! Some denatured alky in a spray bottle can also quickly reduce temps, but it is flammable, so be careful. I've used it without incident.

2nd, the alloy of the Aluminum is very important. Some alloys simply do not machine well and depending on their make-up, you may have a difficult time cutting it no matter what method or tool you use.

3rd, Some bit geometries really like to be climb milled on aluminum and other metals. If your scrap parts look better than the finished part, then change direction (go climb instead of conventional).

4th, The ShopBot is not a metal cutting mill & careful toolpath preparation is a must. Plunges should be ramped into the cut and stepdowns should be no more than .0625" per pass. You should be aiming for a 1.2 IPS speed @ 13,000 RPM. Carpet tape and vacuum, depending on size of part, are usually not adequate. Parts should be drilled using a drill bit specifically for AL. I get these from OBerg Brothers in Maple Shade NJ. I forget what the drill bits are called, but you can drill AL as fast as you want with them & there's no nonsense. Parts should then be screwed down to the table to eliminate any walking. AL is much denser than wood and plastic and vibration becomes an issue on thicker pieces.

It looks like you are cutting 1/4" or 3/8"? You should not be getting that kind of smearing, depending on the alloy. What feeds & RPM are you using?

-B

[john_l]

I didnt have any cooling setup in place yet. I was kinda just going for it. I figured if the bit was done anyway, from the prior uses, it would just fall short at some point. I did keep the dust foot and dust collection running but it was getting hot. I started blowing additional air at the bit with a 14" long blow gun I have. This seemed to help cool it for the first few pieces of these as they cut fine. I think you are onto it... the heat just caught up with me.

I don't really even know the alloy of these pieces. It was some 1/8" alumnum from Harbor Sales that I had left over from another project.

I was climb milling at about 1.1 inches/second, 12,100 RPM (+-), pass depth was .05".

It was throwing excellent curly shaped shavings of about 1/4" long at first. I suspected the heat killed it, just wanted to see if someone else would back me up on that.

This was just a one-off part group for something that I probably won't need again and I got my parts out of it, I just had a little extra cleanup. Shopbot saved me $220 that the satellite manufacturer was charging for these parts.

The (used) SUPER 0 bit seemed to work great on the .040 sheets I was cuting. It seemed like it would never give up with the thin sheets. Is there a milling or machinist type bit that would serve better if I were to ever try this again on 1/8" aluminum?

I used VcarvePro to prepare the file. I just checked and I had not checked any boxes under "lead in" or "ramping".

Thanks!
John

[Brady Watson]

John,
Lessons learned...you cannot use dull bits on Aluminum. The O-flute is good for thinner sheet metals, but a 2-flute High Speed Steel High-helix end mill is best on 1/8"+ thicknesses. They are VERY sharp, CHEAP and are less prone to breakage than a carbide tool. Since they are not as stiff as a carbide tool, they are quieter and give a better finish since this vibration doesn't get transferred to the part.

Holding a blow gun on the cut is really not as effective as making yourself a coolant setup. I've tried the 'manual coolant holder' and got the same results you did. I took about 20min to make mine and it's nice to be able to pull it off the shelf and use it when I need to cut metals.

-B