[ukpete]

Just started working with my new cnc milling/ routing machine and I'm having real problems getting decent results milling aluminium - lots of chattering and poor finish. I'm using a 3mm 2 flute carbide cutter running at 18,000 rpm and cutting 1mm at a pass at .5m/min feed speed. Stock is 3mm thick sheet from the local stockholder, so not sure of hardness. Where am I going wrong?

I'm hand applying a cutting oil as I've yet to source a suitable cutting fluid for the machine's mister system. Any thoughts on a uk supplier of (small quantities) of good quality cutting fluid?

The machine comes from a uk manufacturer Emach (www.emach.eu).

Many thanks,

Peter

[Fegenbush]

Ok, for starters, your RPM looks about right for the material and endmill size. You should be running at least 0.001" per tooth or 0.002" per revolution (36" per min ~ 1m/min), so you need to turn up the feedrate. This all assumes a nice, rigid setup and 6061 T6 wrought alloy. If that's not the case, you need to adjust the speed down to meet the feedrate. You need to know the alloy with which you are working and look up the standard hardness for that alloy. It may not be exact to your application, but it will give you a place to start.

As far as cutting fluid is concerned, kerosene works very well for aluminum. You can put some in a squirt (not spray) bottle and apply it that way. I apologize, but I do not know any machinery supply houses in the UK, but a water soluble synthetic lube is what I use in my mist cooler. Mix it to the instructions on the bottle. $20 a gallon here in the US.

[ukpete]

Thanks for the advice. Once my new carbide cutters arrive (I've broken the previous lot), I'll try the parameters you've suggested.
Peter

[irving2008]

Pete,

At the risk you might know all this stuff (in which case apologies) there is some useful info on this site

If you are buying stock from a UK supplier (who BTW?) he should be able to tell you what alloy it is, but generally if not otherwise specified it'll be 5083 or 6082T6 (there are very few aluminium alloys that dont have good machining characteristics, like 3000series and its very unlikely to be one of those)

Conventional milling (as opposed to high speed machining) says:

revs = 1000 * Vc/(pi * dia) where Vc is cutting speed of material in metres/min

which for most aluminium alloys is 60 - 120m/min giving a spindle speed of 6000 - 12000rpm on a 3mm cutter, so you are running a tad on the high side however high speed machining allows cutting rates up to 400m/min = 42krpm.

Feed rate Vf (mm/min) = Vz * revs * # of teeth, where Vz is feed per tooth in mm.

For most aluminium alloys a good rule of thumb is d/150 for roughing or d/200 for finishing, so assuming roughing Vz = 3/150 = .02 therefore feed rate needs to be around .02 * 18000 * 2 = 720mm/min.

Material removal rate Q in cc/min = width of cut * depth of cut * Vf/1000. You don't say what type of cut but assuming its 1mm wide x 3mm deep (edge milling) Q = 1 * 3 * 720/1000 = 2.2cc/min

This removal rate requires a certain power level

Pc = K * Q , where K is cutting power in Watts/cc

which for most aluminium alloys is 17 so P = 17 * 2.2 = 37W at the cutter, or around double that as input power, say 80W (~1/10HP) so its unlikely lack of spindle power is the issue.

Up your feed rate by 50%, or reduce the spindle speed, and you should get a better result...

but like all things these numbers are theoretical, you need to experiment with your own machine to see what its really capable of... rigidity becomes the key...