View Full Version : Advice needed on feeds and speeds!
12-11-2012, 05:53 PM
I've had my self built router finished for a while now, but its only recently that I've had any time to get use out of it. I built it for milling aluminium parts and it has a 800 Kress spindle. Having no prior knowledge of CNC I just plugged in some modest values for the feeds and speeds and I just never changed them. At the moment I'm cutting at 0.8mm deep every pass, with a 140 mm/min feed rate, usually a 6mm diameter endmill, sometimes 8. I have a pump/tank for flood cooling but haven't really got it set up yet, so I've just been spraying wd40 every so often. The jog rate is 300mm/min and the spindle is set to 2 which I pretty sure means 2,000 RPM. Although this is painfully slow, I was scared of ruining something by going higher so I just stuck with it. However after getting the trial of GWizard, I am now thinking I could be going much faster. However, not really trusting a piece of software I though I might ask around here and see what everyone thought. Like I say its a self built router, fixed gantry, profile rails all round, and it takes two people to lift it. I'll post pics if that makes and difference.
Oh BTW I'm using carbide endmills form Cutwell... http://www.cutweltools.co.uk/files/ww/SM%20A155.pdf. Its not like I know what I'm talking about, but they seem good quality... I know I've cut myself on them all to easily whilst getting parts off the bed etc.
Thank you to anyone who responds with advice :)
12-11-2012, 06:28 PM
hi david, if your anything like me its worth taking what i would considder the easy route and keep an eye on the chips, you will soon get a feel for what a good "chip" is
so your eaither tuning feed or speed based on chip quality
aluminium can be a bitch if its "gummy" in which case WD40 and patience is probably the way to go (a lot of chip re-cutting and can bog down no matter what feed/speed)
if the aluminium is coming away much more cleanly then id just keep an eye on those... idealy you want a nice consistant chip with a bit of weight (thicker than tin foil!!)
at 2000rpm, single flute carbide my feed would be closer to 200mm/300mm depending on what the chips look like
if your tool has more flutes your speed needs to be a bit higher than 150mm.... maybe 300mm plus
be brave and be prepared to lose a tool :).... it may be worth having a look at the single flute carbides (ebay) nice n cheap and work well in all sorts of materials
I know I've cut myself on them all to easily whilst getting parts of the bed etc.
join the club :)
12-11-2012, 06:30 PM
Try (Constant Surface cutting speed, around 300 roughing, to 400 finishing, * 318.3) all over the cutter diameter.
So try around (350*318.3)/8 = rounds up to around 14k rpm.
so with ur rpm speed u need the appropriate feedrate, this is speed in rpm * no of teeth (or flutes same difference) * chip load per tooth (0.04mm finishing to 0.08mm roughing)
So say 14k * 3flutes * 0.06 = 2520mm/m
That probably wont help you, this might: Speeds and feeds - Wikipedia, the free encyclopedia (http://en.wikipedia.org/wiki/Speeds_and_feeds)
However those values are for HSS, your are using carbide so see above?
13-11-2012, 11:48 AM
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.
13-11-2012, 12:55 PM
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
14-11-2012, 11:47 AM
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.
Powered by vBulletin® Version 4.2.3 Copyright © 2016 vBulletin Solutions, Inc. All rights reserved.