Official Luthiers Forum!

I've never had much luck with dry machining aluminum. Even using mills with aluminum geometry, lowest router speed (10K), fast passes and lots of air I still get a little too much galling. What's the secret?

Don't dry machine it?

Seriously, though I also disbelieved it when I started, dry machining aluminum is a bad idea unless it's so thin that it's sheet cutting or there is no other option and you're a pro shop. Get a thick cutting fluid or some goopy tapping stuff like Anchorlube and dip the cutter in it every minute or so. If it still galls then your feeds and speeds are wrong.

Filling a small squirt bottle (like a window cleaner bottle) with a non gross lubricant and giving it a shot every 30 seconds works, too.

Or you could make a fogless coolant mister, using only drops of coolant per minute. Threads about it on CNCZone. It's not a hard project if you make it from brass air fittings and copper tube- you can solder it all together!

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Your question can't be answered without addressing a specific set of circumstances. Dry machining is done all the time but machine rigidity, mass, feed rate, spindle speed, chip removal, cut depth, material type, cutter selection....nothing but variables.

Dry machining of metal should only be attempted with rigid machines....which excludes virtually everything available in the low end category of cnc machines. Galling occurs for a number of reasons which are all tied to an uneven chip load. Vibration produces an uneven chip load. The more vibration, the more uneven the chip load. When a cutting edge does not engage material correctly it will quickly lose its sharp edge. To cut through material is better for a sharp edge than glancing along side of it because right at the very tip, where the cutting edge is microscopic, it's better for there to be material on both sides of that tiny area in order to support and sustain that edge. Think of it this way. If you are trying to break the tip off a tall, skinny triangle, will it be easier to do this by pushing down on the top of it or by applying pressure to the side of it? Of course....by applying pressure to the side of it. If you can visulaize a cutting edge as this triangle you can see that cutting through material is better than glancing along side of it.

With vibration in the system, one flute may cut pretty well while another may glance off the material.

When each chip coming off each flute is the exact same size....you have minimized vibration. When the machine itself hasn't enough mass or mechanical accuracy to avoid vibration, the result will be uneven chip load. Cutting fluids provide lubricant which allows a flute to cut through the material with less pressure, consequently reducing the amount of side pressure on the cutter, consequently reducing the dynamic vibration within that system. But coolant, ideal feed rates, and perfect spindle speeds aren't going to eliminate vibration when the machine has no mass and doesn't have good rigidity.

Anyway...the trick is to get each flute to make a clean, full cut, produce a consitently sized chip, and then eject that chip cleanly without recutting it....and I think that's going to be close to impossible when cutting metal on a light machine. These light machines can cut wood because the side loads on the cutter cutting wood is a small fraction of what is required to cut metal. Your best odds at doing this will only happen when you use the recommended chip load for that cutter...obtainable with the correct feed rate, spindle speed, and cut depth...all possibly obtainable from the folks you bought that cutter from. But don't hope for too much here.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Thanks Bob. I'm looking at a new to me machine that's a whole lot harder to clean up for wood use than my old one.

Stuart, that's a great description!

Feed Speed =RPM *n * Chip Load..where n is the number of flutes....

You can get some typical chip load numbers from the manufacturer's who make the tools...

For example, here is some VERY good literature:

http://www.vortextool.com/images/chipLoadChart.pdf

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

What kind of machine, and what do you mean by 'clean up for wood use'?

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob...I'm guessing here, but it sounds like a mill that has lots of oil and gunk on it!

Mike

Stuart

I currently run a biesse point to point machine with vacuum blocks on, could this machine do aluminium work on it is used for milling wood on but do you think i could machine on it. do you think i would need to have a stronger hold down system on the machine.

Thanks in advance

Jeremy

A used Fadal 4020.

So you have one of these?....a big, heavy machine that's likey to be fairly rigid and accurate? Or that's what you're thinking about buying?

You'll be able to cut just about anything with that Fadal but only if it's not too old and tired.

In any case...let us know what the typical scenario you are experiencing galling with. Cutter, # of flutes, type of cutter material, type of aluminum, feed rate, spindle speed, and cut depth.

Using a Haas VF-4, a two flute, carbide, 1/2" cutter at 40 ipm, 5000 rpm, a cutting depth of .1", and a stepover width of .25"....there shouldn't be any need for coolant provided you are not taking super long passes and heat doesn't build up too high. For instance, using those numbers I can take a 12" long cut on 6061-T6 without building up too much heat. That's a shoulder cut where the chips get thrown away from the cutting point. If cutting a groove the chips will not all get thrown out and this problem will become worse and worse as the groove deepens.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

If this is the machine:

http://www.youtube.com/watch?v=pZLYvTfDw50

Then no.....this system is designed to cut wood....from the sound of it, it runs at very high rpm and the holding system presumes almost no side loading of the spindle. There is a fundamental difference between machines designed for wood and metal. A machine designed to cut metal WILL cut wood whereas a machine desiged to cut wood WILL NOT cut metal due to the presumption of low side loads on the cutting tool. The harder the material being cut....the more important rigidity becomes. Rigidity is controlled through machine mass, machine accuracy, and a thorough grip of the material being cut.

A piece of metal would probably fly off this thing immediately. The risk to your spindle would be pretty high if you were to try this. This also assumes you can mount the right cutter, have the appropriate spindle rigidity, and use the appropriate spindle speed (about 5000)....which doesn't look likely.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Stuart, that statement is not necessarily true! Ask me how I know! A large foot print 9ftX12ft kit built router will in fact cut steel ibeam at 300ipm with a .500" two flute to a depth of .100". At least for a short period of time, then the bit seems to change it's geometry....quickly!

I almost posted a reply to your earlier post about rigidity. Everything you said is true, and in my case proven. The steel was of course accidental, or stupidal ( word??) but I have tried to cut alum with my router spindle turned down to 5k rpm and even then I could not move the machine fast enough to prevent galling.

Mike

That's a tiny, short, slow cut in ideal chip clearance conditions with a low spindle speed and a chip load that's very low even for that speed. The advice it's backing up is flat out malignant to give out to a newbie. Trying to cut aluminum dry, in realistic conditions, is going to cost you cutters and maybe even damage your spindle bearings if it happens just right. I know this because I mill thousands of pounds of aluminum every year for clients, but I will have an MASc with a thesis involving machining research to pad my resume come January Don't play with other people's money.

Aluminum galls because it's sticky and it has a low melting point. The tiniest bit of lubricant, and careful track of heat buildup and chip clearance will get rid of this. Unless I'm doing deep pockets, in which case I'll usually turn it up, my lubricant usage is measured in drops per minute. If you stick a finger in front of my coolant nozzle, you have to wait a few seconds to see it get wet. If I run the cutter dry, with the same parameters, it's got about 30 seconds to live.




I think it's doable...Taylor has something like 50 of them and mine's doing just fine:


Take the flood coolant lines out and route air to them, then you can use them to blow chips off your work. Put a roof on the machine, cut around the spindle, to keep the dust from flying out the top. If you want to use dust collection, then you can cut holes in the bottom of the enclosure and put flanges on them as theirs and mine are set up, but in retrospect I'd recommend putting the dust collection in the top to catch the light dust and just shoveling out the enclosure when you've got 6" of heavy chips in it. Use mist coolant for metal-cutting, and wipe down the table and spindle head with a rag and acetone between cutting metal and wood - ten minutes if you're both meticulous and lazy. I can be bribed with a nice piece of wood to make you a fogless mister instead of paying a few hundred for a FogBuster . You can see mine folded up on the right of the spindle in that pic.

What year is it? I'd try to get one with metric ballscrews if you can; it's worth the extra dough, as that's pretty much the most valuable part of the whole machine and the hardest to change. You can replace motors or the control easily enough, but the inch screws are much smaller (and thus slower) than the metric ones. I believe they switched over in 1994 but it's best to double check. If you retrofit a good controller to a metric screw machine (cheaper than you think), you can get one of those machines -really- cooking.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

It's a 1988. Not my first choice but I've been looking for '94-'98 vintage machine for a couple of years and for my budget there hasn't been anything pop up.

I'll likely take you up on that mister. What kind of wood do you like?

Slightly off topic. Any thoughts on where to get tool holders on a tight budget? Used? KBC?

That's right.....on a big, heavy Haas...as I said. Try those conditions on a $4000 cnc router kit and see what happens? Is that what you think I'm saying? Read the thread again. If he gets the Fadal...then I gave him a safe starting point...a shoulder cut with a non-aggressive chip load.

Of course....those conditions will overwhelm a machine that isn't designed for the side loads required to cut metal. You should conclude that I'm trying to steer people away from experiementing with the dry cutting of aluminum on machines that are not designed for cutting metal. I'm not a saint and I've been known to not thoroughly read a thread or understand a guy's point. That's easily forgivable.

...but what's this?



I think you meant to say "malicious". It's not a tumor, Bob. In either case, that's a hell of a thing to say about someone you don't know very well. Do you do that often? I'm here to learn from those I can learn from and to help those I can help. I'd like to do that as humbly as possible...without doing battle.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

http://www.discount-tools.com or Maritool http://www.maritool.com. They have pretty much the same prices you'll get off eBay unless you're very patient and persistent. I'd go with whichever has more stuff you'd also like to buy at the same time, which would usually be Maritool in my case.



A decently solid router could remove more material than that, and faster, with lubricant. Without lubricant, no machine can remove a whole lot of material much faster- because it isn't an issue of machine dynamics, it's an issue of chip galling. It could be his machine is too weak as well, but his complaint wasn't about the cutters bogging down or massive amounts of chatter shaking his machine, it was about galling.
...



Definitely meant malicious, after the prefix it all goes to junk in the middle of the night. Probably a strongish word, but given the option to give no advice at all and then choosing to give poor advice is ignoring the indifferent option to choose the harmful one.

You've given a lot of good advice on this board, and I've gained a lot of respect for you based on some of the things you said, but that just makes it worse when you give bad advice. The humble thing would have been to directly say that it's, in the broadest terms, a bad idea to machine a material that galls extremely easily without lubricant. Throwing down a bunch of woo about machine dynamics, then suggesting he failed because he just didn't understand the magic parameters to cut aluminum dry, is neither humble nor helpful. The only reason I said something overtly is I know that you're tough enough to take it, and smart enough to know better.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob, it's starting to seem that being "humble" means agreeing with you. Well...I don't agree with you, Bob.

I machine dry aluminum on a fairly regular basis without galling. Something has to explain that. I disagree with you. I think there are a number of things that more explain galling aluminum than a lack of coolant....machine rigidity being the primary factor as well as the most likely factor in this scenario since most of these guys might be using or considering a less expensive machine that will likely not be designed for metal. Tool sharpness and concentricity play a crucial role too.

Nor did I suggest that people use the parameters I posted to go out and apply them to their machine...which you've now TWICE asserted incorrectly. I'm wondering how you could actually read what I wrote and come to that conclusion. That Fadal he's thinking about compares to the Haas such that the numbers I gave him ought to produce a gall free cut....with 6061-T6.

By all means...use coolant when you can. Sheldon's post implied that he either couldn't or didn't want to. I'm telling him that Fadal will do it and a lesser machine won't.



That doesn't quite explain your behavior, Bob.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Nah...I'm done. This is like the Twilight Zone.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

well, anyway getting back to the op... what type of aluminum things do you wish to cut?

some things to consider...
-try coated tools: ticn or diamond. tin galls quickly in aluminum when going dry. 3 flute niagara a337's are cheap and durable. one does not always need carbide and with a shifty machine like a router pressed into metal cutting service you risk chipping and wasting the expensive carbide tool almost surely due to lack of rigidity, lateral and axial float

-minimize tool overhang. keep the tools up close to the spindle. this helps with the rigidity issue. don't use overly long tools either.

-a cold air blast goes a long way on open milling and some pocket milling when going dry.

-drilling dry is more difficult but do-able provided you reduce friction (with a coating) and spalling/metal pick up by proper geometry and feeds/speeds. peck increment is important. go with g73 on shallow holes up to 3x diameter and g83 for deeper. slowing down the retract rate will help in getting all of the chips out of the hole before slamming the tool back into a pellet of packed chips. try to start out conservatively on the peck increment. i prefer about 25% to 33% of drill diameter to start. i also prefer drill points at 135 degrees because i find that they fold and break up chips quicker which helps in evacuation.

-some formulae: rpm= sfpm x 3.82 / tool diameter. feedrate= rpm x chip load per tooth x # of cutter teeth. these formulas work and when used with the cutting tool mfg's data are you best chances for success. a lot of people go with a "rule of thumb" approach. for example "100 rpm at 10 ipm" ime this negates a competent cutter manufacturer's r&d lab and the capital dedicated to developing what works best for their tools. some years ago we conducted experiments with sandvik coromant on a line of their carbide inserts. without fail, when run at the prescribed conditions, these tools preformed as stated to within +/- 4~5 mins of tool life. the sample size was about 1100 inserts or so if i recall. it pays to take advantage of a large cutting tool manufacturer's experience.

-material selection. copper based 2000 series alloys suck to machine. they are so gummy it's like machining a candy bar. try to avoid it if you can. magnesium based 6000 series in t6 condition and zinc based 7000 series are far better choices with 6061 t6 being the dominate selection.

-a Fadal 4020 from 88' ? this will work. have the machine checked out before you buy. the spindle taper should make at least 75% contact or it'll need a re-grind. i personally don't like the fadal and words like "large" and "heavy duty" don't apply to haas ime. i don't care for the fadal spindle bearings because they are smaller in size then normal to account for the tool changer notch on the spindle snout. i don't like their ballscrew/way cover arrangement as it isn't very protective and the early model's had poorly ground threads. i don't like the control on the 4020. it's balky, slow and having the machine's origin planted in the middle of the table is annoying -but i've used worse and wouldn't turn one down for a good price. many people use them and are happy. like taylor, olson, and carvin for example.

imo if you can though, try to get a haas. they are sufficient for cutting wood, plastic, and aluminum. their control is one of the best and easiest to use currently -even the old ones. haas factory service is some of the best in the industry where fadal is owned by thyssen-krupp and i hear service isn't exactly what it could be. haas is run by gene up in oxnard ca. and they are very responsive to users of both old and new machines alike and their factory service outlets are numerous.

Arie,

that is a GREAT explanation! You are right, staying true to some of the formulas for initial cuts, will work....like others have said here, using coolant is always a good idea, but if you achieve an optimum chip load, where the chips ejected actually carry away heat, it can be cut without....

For laughs and giggles, do a search on youtube for cutting aluminum with a cnc, and there are many folks who are doing it with a home build machine...some as you can see, get good results, while others, galling is evident...

Nothing like experimenting!

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

Rigidity is not the primary factor, and it's easily proven by running a low rigidity/chattery tool with coolant and a rigid tool without. The chattery but lubed tool can leave an amazingly horrible looking cut without galling while the dry cutter often won't make it to the other side of the test cut at all. Get an extended length and a stub length cutter and try it for yourself. I'm all for differing opinions coming from different experiences, but facts aren't subjective.

Chips ideally take away most of the heat from a machining operation, but the way that heat's created is why aluminum is so much trouble. The heat's a combination of compression in front of the tool and friction along the tool edge, which brings aluminum easily up to its melting point as it's being pushed over the edge. That quickly leads to a built up edge, galling, and then cutter wadding. Most of the basic machining theory people get is based on steel cutting, where speeds and feeds can solve all problems, but it's a whole different ballgame with material properties (ferrous) steel doesn't generally have like work-hardening and galling.

Fadal service doesn't exist at all anymore, or might as well not exist. They canned most of their top support personnel after they closed the factory. I think they're just coasting along until they're not breaking any support contracts and then it's all over. The third party suppliers have really stepped up, though. A Fadal or a Haas isn't big iron when you're comparing it to Mori's, but they're pretty hefty when the status quo is an aluminum extrusion router.

The upside for Fadals now is that the prices are dropping hard due to the lack of support prospects, and they're really good machines if you retrofit the controller to something nice. Mine can cut smoothly at its old rapid after a retro, though I'd probably cook my ballscrews and motors running at 600IPM all day. The clunky electronics/control design makes retrofitting them a lot easier than I'd expect it to be on a Haas. The rear Y axis way cover design is atrocious. While the brain of the controller is weak, the interface is still my favourite: independent and always on feed, speed, and rapid override pots are something that should be on every machine. You can actually tune feeds and speeds by ear.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

of course rigidity isn't the root cause. who said it was? it is a variable but it's a little bit down the list though.

"Most of the basic machining theory people get is based on steel cutting, where speeds and feeds can solve all problems..
-well no, not true. speeds and feeds are calculated in part upon the uts of the material expressed in kpsi at plastic deformation. which is different for each material.

then there's the pixie dust...

That would be Stuart.
In bold italics.





Did you just disagree with my assertion that proper speeds and feeds are usually the solution to steel machining problems by saying that improper speeds and feeds are usually the problem when machining steel? I mean on a machine that can actually push a cutter through steel in the first place, of course. The numbers only get you part of the way there, whether you're trying to use just the Merchant equations or if you go all the way to specific energy and heat diffusion craziness and numerical methods...and then empirically derived stability lobes ruin all your good calculations[1]...and the next thing you know you're burning up 1100 inserts to see where the math went wrong

1: Though I think they're going for the glory now in trying to do a massive number of harmonic measurements on different machines and tools to try and make a predictive database

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

bye bye