Advice needed on feeds and speeds!

[lateAtNight]

Thanks to you both for replying,
I noticed both of you talk about feed speeds and RPM but not depth of cut? According to GWizard I could get away with a 2mm DOC, 300mm / m feed rate, and an 8000RPM spindle speed, and that won't come even close to using the the 800w available on the spindle. Sound reasonable? I'll take your advice and pay attention to the chips. At the moment they are kind of like dust, reasonable size but they weight nothing... thiner than tin foil.

I wouldn't mind loosing an endmill in the name of experimentation... its more ruining the bearings in the spindle or something.

Thanks again,
David.

[blackburn mark]

deapth of cut with a 6mm tool would be dependant on your machines rigidity
with a router we tend to feed a shallow cut quicker rather than deap one slower... if that makes sense

if your chips are like dust your tool life may be vastly shortend as it will be doing quite a bit of rubbing and only taking a cut on every other revolution or worse

the ideal is to be taking a consistant healthy chip... if your aluminium is gummy it can be really hard to acheive this and plenty of WD40 and an old tooth brush to clear as much of wast as you cut is as good as it gets

it this stage it may be worth being really experimental with your speeds and feeds and eccept any tool loses as part of the process of finding the sweet spot

being conservative can damage your tool just like being agressive

in my opinion, if you have an idea of a healthy chip it doesnt matter what your cutting, youll have the ability to nudge the feed or spindle speed on the hoof and over time youll start to add your knowlege at the g-code level

[Jonathan]

According to GWizard I could get away with a 2mm DOC, 300mm / m feed rate, and an 8000RPM spindle speed ... won't come even close to using the the 800w available on the spindle. Sound reasonable?

Yes, it doesn't take as much power as you might expect. Also bear in mind that the output power available from the spindle will reduce with speed, so at 8000rpm you will have less than 800W available. The 2mm DOC suggested by Gwizard is most likely limited by the tool deflection (bending, snapping), so consider that to be a limit. You will more than likely first be limited by the rigidity of the machine.

As mark has said - use the calculated feedrate as that's bound to be close, then start with a low depth of cut and gradually increase it until you find the limit of your machine, or the tool. You'll almost certainly be better off with a 6mm single flute cutter (look on eBay), since having only one flute means there is more room for the swarf to eject. This helps prevent it building up on the tool. If you do get those cutters then use 13000rpm and 600mm/min. Again start with a small depth of cut and work up.

Also it's helpful to remember that the rpm is inversely proportional to the diameter and varies with the type of cutter - so in general it does not depend on the number of flutes. That means a 6mm 2fl cutter should be run at the same rpm as a 6mm 1fl, assuming they are both carbide. However the feedrate scales with the number of flutes (since it is dependent on the chipload), so you should run a 2fl cutter twice as fast as a single flute cutter.

Do you know what grade the aluminium is? If it's something like 5083 you'll find it much more difficult to cut than 6082 for instance.