Feeds and speed when milling Aluminium

Hi,

I've been doing some milling in aluminium with my DIY-CNC router. The router is a 1.2x0.6meter mill with a 2.2kW water-cooled spindle. The axes are driven by quite powerful Nema23 380oz/in steppers.

It's very hard to know the correct feed, and the correct spindle speed when milling. Also it's hard to know how deep I can cut . So when Im doing it wrong, the flutes gets filled with aluminium and I have to pause to remove it.

So here is my questions for aluminium milling:
1: Is there any rule or guidelines to how deep one should cut (as long as the spindle is up for it)?
2: Is there a way of calculating the correct feed and spindle-RPM?
3: When the flutes get packed, should I turn up or down the feed or the spindle RPM?
4: Is there such a thing as too much cooling liquid (except for the mess)?


As for point 4: Im now having cooling liquid on a spray flask, and spraying from time to time (maybe every 10-15 seconds). Is this OK, or I'm I using too little?


Thanks for any and all answers! :)

Download this to help you figure out your options: GWizard: A CNC Machinist's Calculator

It's difficult to answer your questions properly on a DIY router as vibration will be a big factor in feed & depth of cut. The spindle may be up for it but frame flex, precision tolerance, and required surface finish will contribute to the outcome. I will attempt to provide some info, I'm not the last word on your situation.

1) I always like to take at least 2 cuts in an operation, one for rough and leave perhaps .25mm for the finish cut. Chip evacuation is critical for any cut, otherwise you're re-cutting chips. Should chips clog the flutes the new chips have to push the old ones out of the way or they pack up in the flutes. This can greatly affect the feed rate, finish, and accuracy of your work piece. This is particularly critical for aluminum as the chips tend to stick to each other as well as the cutter. The softer the aluminum the worse it does this.

2) Sure, you can use a ballpark estimation by any of the calculators that are on line. Here's just one Milling Speed and Feed Calculator

3) If you're packing the flutes then you need to see about chip evacuation first before you change anything else. Compressed air or flood coolant, although messy, are good solutions to begin with. If you can't get enough air/coolant in to clear out the chips then there's too much material being cut. When I have a speed/feed calculated then I proceed to find out if I can clear the chips out of the way. Usually I'll back the feed down or shorten the depth of cut so there's less material coming out, slowing down the spindle speed is for when vibration is causing a squeal from the cutter. Even how solid your work piece is held to the machine can make a big difference.

4) I've never had a cut where too much coolant did anything but create a mess. I suppose if you had a very small cutter and you had very high pressure coolant steams it might cause some deflection but that's not likely. A bigger factor is the type of coolant used. Milling speeds for aluminum can be very high without risk of burning up a cutter but chips welding themselves to the cutting edge can prevent any cutting from happening. I've seen cutters that were deflecting and pushing the material because it couldn't cut due to material being welded onto the cutting edge. For aluminum I like to use something made for aluminum. I've used kerosene, mineral spirits, and even strong soapy water when I had nothing else. I've even held a bar of soap to the cutter for a moment before running the cutter into the material if it's a short cut. Some oil thinned with petrol can even be used. I prefer using a thin fluid that is more a lubricant than a coolant when milling aluminum. Since you're using a spray bottle (nothing wrong with that either) then if you can hook up a small stream of compressed air on the leading direction of the cut (blowing chips away from the cut) I'd spray with the air stream and use enough to clear chips off the cutter. I would guess that every 3-5 seconds is a minimum for a spray bottle. Flooding the cutter will produce better results, you'll have to deal with the excess liquid but it should give you better results.

Hope this helped.

Thanks for the link mcphil - I've signed up for a trial.

Thanks roninB4 for quite some insight!

So I should not worry so much about feed and spindle speed then, but rather keeping chips away. This is somewhat a problem atm as I dont have compressed air (another thing that I need cash for...). Now I just spray chips away with my coolant.

Is there a downside of having too little feed (or too fast spindle) other than the longer milling time? I believe I've read somewhere that if the feed is too slow, the tool will gnaw on the stock instead of actually cutting. Is this correct?

So if I understand correctly; the packing of flutes can come of two factors: 1: too much chips not being properly evacuated; and/or: 2: too hot, which melts the aluminium to the cutter.


Thanks again for very insightful answers :) It's much appreciated!!

1: Is there any rule or guidelines to how deep one should cut (as long as the spindle is up for it)?

That is about it, don't stall the spindle, don't stall the steppers and don't break the tool. As a general rule stay less than about 1/2 cutter diameter deep when cutting full width but go deeper when the cutter is only partly engaged. And do half or a quarter of this with cutters less than 6mm.

2: Is there a way of calculating the correct feed and spindle-RPM?

Feed is based on the cut per tooth and the spindle rpm, spindle rpm is based on material being cut and the cutter.

With carbide cutters aluminum alloys can easily be cut at 1500 meters per minute which corresponds to a very fast spindle rpm on a small cutter so most likely the machine can be run at full speed. When High Speed Steel (HSS) cutters are used the rpm should be about 1/3 that used for carbide.

As mentioned feed depends on the cut per tooth; the distance the tool advances per revolution. It also depends on the depth of cut and the width of cutter engaged in the metal. At depth of 1/2 diameter and full width cutters above 10 mm can normally handle a cut per tooth of about 0.5% of the diameter; smaller cutters need to be scaled back toward 0.1%. When the full width of the cutter is not engaged in the metal the feed can be scaled up because the actual depth of cut per tooth is less than the amount the cutter advances per revolution. The rate at which the cutter advances is simply the feed per tooth multiplied by the number of teeth and the spindle rpm. For example 0.01 mm per tooth for a 2 flute cutter running at 20,000 rpm is 0.4 meters per minute.

3: When the flutes get packed, should I turn up or down the feed or the spindle RPM?

Yes, No and Maybe.:D Very often chips packing in the flutes is a result of no lubrication and/or too many flutes. Always use 2 or 3 flute cutters with a high helix angle for aluminum. Fewer flutes means more space for chips and the screw like action of the helix tends to pull the chips up out of the cut. Of course blowing or washing the chips away with air or coolant is always a good idea. Too much feed or too low rpm can enhance the tendency for chips to pack because the chip is thicker. Soft aluminum alloys, 'low temper' or annealed are terrible for packing.

4: Is there such a thing as too much cooling liquid (except for the mess)?

Not really but often simply spraying, or brushing coolant on the surface to be cut, is adequate. Coolant really becomes essential for deep, full width cuts running at the top end of the feed range for the cutter, rpm and material when cooling is as important as lubrication. To reduce the mess on an open machine the best is probably a mister that blows coolant and air to provide cooling, lubrication and remove chips. These can also create a coolant aerosol in the air so wear a suitable grade of breathing protection.

Quote:

---

Originally Posted by Vaffel

Thanks for the link mcphil - I've signed up for a trial.

Thanks roninB4 for quite some insight!

So I should not worry so much about feed and spindle speed then, but rather keeping chips away. This is somewhat a problem atm as I dont have compressed air (another thing that I need cash for...). Now I just spray chips away with my coolant.

Is there a downside of having too little feed (or too fast spindle) other than the longer milling time? I believe I've read somewhere that if the feed is too slow, the tool will gnaw on the stock instead of actually cutting. Is this correct?

So if I understand correctly; the packing of flutes can come of two factors: 1: too much chips not being properly evacuated; and/or: 2: too hot, which melts the aluminium to the cutter.


Thanks again for very insightful answers :) It's much appreciated!!

---

Speed and feeds are important but you can arrive at a starting point by using the calculators for this and making small adjustments per the application. The speeds and feeds should be calculated before you ever turn on the machine.

Geoff brings up a few good points that I left out, the number of flutes a cutter has can make a difference. If you're not taking a lot of material out then the number of flutes isn't a concern, I've used 4 flute cutters when finish milling pocket walls. But if you're having trouble with loading up the cutters then you really should be using a 2 or 3 flute (2 is better) cutter. You should also look at the depth of the flute if these are re-ground cutters. You want to have as much space for the chips as possible when removing large amounts of material. Geoff also brings up the high helix type of cutters, they are better than straight flute or standard helix (only for aluminum). Since you haven't mentioned what type of cutter or the material the cutting edge is made of some details may be overlooked. If there's too little feed you can "work harden" some materials but not aluminum. Unless you're way out of the ball park I wouldn't worry about too much heat either. When I used the term "welded" I probably should have used the term "bonded" when I wrote about the material sticking to the cutting edge. This is a bigger problem with carbide than HSS as prying off the aluminum from a carbide cutter as there's a chance you could chip the edge of the carbide, less likely with HSS. This is just my opinion but I see no advantage to using carbide on aluminum. If you do use too much feed or too low an RPM and the cutter gets packed up you could snap the cutter off. Look up what your speed/feed should be, adjust your settings, and try to use either a spitter/mister to clear out chips, using an appropriate fluid. If you want to see what difference it makes just set your spray bottle to stream (instead of fine spray) and continuously soak during the duration of the cut. If it works better then you know you're on the right path. Post up what you do, others may be having similar trouble.

Thanks both of you :)

Well, I only have one high helix end mill (4mm). Or at least I believe it's a high helix. It looks more like a screw than the others, like its much more twisted.

However, I haven't tried this one yet (but I will next time).

I've mainly been using carbide 2 flutes in aluminium. These are bought off ebay from asia, and are probably not of very high quality.

Yes, I'm using the spray bottle on stream, not on mist! However, I havent tried soaking the stock yet :)

I'll probably try some more later today, so I'll get back to it!

By soaking I should say that you use a constant stream of cutting fluid to help wash the chips off/out of the cut path.

Sorry for any confusion, my English isn't so very good sometimes. A 2 flute (3 is ok too) is more important than it being high helix (that has more "twist"). You can also use a small brush to help drag chips out of the cut path but I'd be very very careful with that. I've used this to help but you can easily get the brush caught in the cutter. Not a good thing.

Quote:

---

Originally Posted by Vaffel

Well, I only have one high helix end mill (4mm).

---

I do not know if that is representative of the endmills you generally use, but many people think "small machine -> small endmill". Not so. A machine with a small 1hp motor should be able to handle a 12 mm endmill no problem. The larger endmills are much more forgiving. And because of the much higher SFM they enable a "small and slow" machine to get much closer to good cutting conditions :)

Sorry if you already know this :p

EDIT: oh just saw that you are using a router as opposed to a mill. Nevermind what I said :D

Quote:

---

Originally Posted by mcphill

Download this to help you figure out your options: GWizard: A CNC Machinist's Calculator

---

Looks like downloading the app is free but registration is not.