Thread: Aluminium cutting
I wonder if someone could check my setting for cutting aluminium as I keep breaking end mills. The last time I had this settings. The aluminium is 6082 T651 18mm thick I am just using this to test. I'm trying to pocket out a 25mm diameter hole only 6mm deep and I'm only getting to half way round the second pass.
The bit is a 1/8th single flute carbide bit, the depth of pass is 1mm RPM is 15000, chip load I have as 0.003 which I workout as 1142mm per minute feed rate plunge rate I have as 126mm per minute, the coolant I am using it duck oil its like WD40 but does not evaporate like WD40 and is a better lubricator.
Recap. Aluminium is 6082
Bit is 1/8th carbide single flute.
feed speed is 1142 mm/per/minute
plunge rate is 126 mm/per/minute
spindle speed is 15000 rpm
depth per cut is 1 mm
step over is 30% 0.952 mm
chip load is 0.003
There must be something in there where I have picked up wrong for working out feed and speed.
This is how I worked out my feed rate.
Feed Rate = RPM x number of flutes x Chip load.
Which gave me 45 I/P/M then to change to metric I divide that by 39.374 which gave me 1.142 metre which is 1142 mm. or multiply 45" by 25.4 which is 1143mm
Or is this all wrong.
Well take this with a pinch of salt but Gwizard tells me that at 15000rpm 1.4 doc 279 mm/min plunge 276 mm/min and 24000 rpm 446 mm/min.
I am not an expert by any means on using the calculator so please wait for another opinion. ..Clive
I've only been cutting wood but from that experience I would say your spindle speed could be lowered and the feed rate is way too high. As it is it's trying to cut 3/4" a second which does not seem right.Spelling mistakes are not intentional, I only seem to see them some time after I've posted
I have tried a slower feed rate but it blunt the end mill to a point it was not cutting but I cant remember the setting since then I have started to keep a note of what I have been trying. If I took the spindle speed down to 10000 rpm then the feed rate would be 30inch a minute or 762mm per minute, at a chip load of 0.003 but if my feed rate is to fast at 15000 rpm at 1142mm per minute should it not be the case that at 10000 rpm at a feed rate of 762mm per minute still be wrong. is there something wrong with the calculation that I have found or is it the chip load that is wrong for a 1/8th single flute end mill. also how slow can you take a water cooled 0.8kw spindle before it would stall when cutting.
Are you roughing or trying to get a decent finish - there's quite a difference between the two I've found.
For roughing I am using mostly a 6mm single flute carbide end mill using 16,439rpm and somewhere between 550 and 650 mm/min - when this is right and the tool is sharp its almost noiseless when roughing through 6082 T651. The lower feed rate seems to be better when the tool is slotting (6mm width) and higher when running at my normal 45% step-over. Also that's all at 2mm DoC - I've tried deeper at 3mm which is OK'ish and much deeper at 5mm but the latter was shrieking.
I'm using GWizard, which now has a gantry router setting and this is on either the 2nd or 3rd setting (highest kills tools and lowest is resulting in "rubbing" i.e. there's a lot of crap not being cut and being "pushed" out of the way.
Finishing paths are a different ball game as the very low "step overs" mean you can get chip thinning i.e. heat which needs getting rid of and also means high feed rates (3000mm/min+) and if that runs into a slot condition goes bad very quickly.
Hope that helps and I'm always on the lookout for experience in this, as getting in the "window" of feeds and speeds means the difference between nice, acceptable and ruined parts - especially with gantry routers.
Oh also a misting/flood system is a must IMHO for aluminium, as is paranoid blowing out of chips with compressed air - I have had everything cooked right before and snapped a tool just from clogged chips in a slot before.
Hope that helps.
PS. See my Youtube channel for some examples of pocketing 6082 T651.
Your chipload is too high. For single flute tools, these are roughly the settings I use for cutting aluminium:
Ø1/8", 24000rpm, 500mm/min
Ø4mm, 18000rpm, 600mm/min
Ø6mm, 12500rpm, 600mm/min
Ø8mm, 9600rpm, 600-700mm/min
...then tweak the rpm until it 'sounds right'. That should get you close enough. With limited coolant I'd be inclined to lower the rpm and feedrate proportionately - soo keep the same chipload but run slower.
Here's a video of my machine cutting with the same tool (@2:14):
The Following User Says Thank You to Jonathan For This Useful Post:
Chip load is wrong it should be more like 0.05 not 0.003. As a rule of thumb for chip load for roughing(50% stepover) divide the cutter diameter by 80. For slot cutting divide by 120.
15000rpm would give feed rate around 800mm/min with DOC 50% cutter diameter.
There are so many variables to working out speeds & feeds and the ridgidty of machine plays large factor so it's very difficult for anyone to work out F&S for someone else.
Also when getting into smaller cutters the material plays big part because while in theory the Grade of aluminiun should mean uniform hardness it doesn't and it's not uncommon for the same grade of aluminium to cut differant from batch to batch and even from same sheet.!! Only experience can help with this and unfortunatly this does mean wrecking a few cutters to learn.!
One thing you don't mention is how your entering the material.? You mention plunge rate and this makes be think your plunging straight down into the material.?
This is bad for tools and Esp single flute cutters so it WILL be knocking the edge off the cutter resulting in more heat.! . . . HEAT is the enemy and you want to aim for chips that are very hot but cool/warm material and cutter. When you have it corrrect you'll get a better idea of what I mean becuase the chips really burn when they hit you.
So when entering material either pre drill a hole and plunge into this. OR use ramping or spiral entry stratergy. Never plunge aluminium with a single flute cutter as it just kills them.
Loads of air and coolant are a must when slot cutting with small cutters and even when stepping over 45-50% they still need good chip clearing to prevent heat build up from chip re-cutting.
Edit: Bugger didn't see Jonathan had beat me to it but never hurts to get it said twice. .Lol . . . .. . Oh and I think Jonathan ment to say it's much kinder on spindle to Ramp rather than "Not Ramp".!
Last edited by JAZZCNC; 21-04-2014 at 09:27 PM.
I have just been trying to get a rough pass, I have never tried a 6mm carbide end mill as I don't have many and I'm sure the ones I have are only for wood, but I will order some and try, could you please tell me how to find you on YouTube, as I would like see your channel, I must have watched hours of cutting aluminium on YouTube and you can hear some of there end mills screaming. then you find one that it looks like it was cutting butter with a hot knife and that's where I want to be but am having a hard job finding the right information.
I have watched a Dennis martens cutting 6040 aluminium but there is no information about how he is doing it feed and speed plunge rate etc.
By Tenson in forum Tool & Tooling TechnologyReplies: 22Last Post: 29-08-2016, 10:41 PM
By Pointy in forum Metalwork DiscussionReplies: 5Last Post: 05-05-2014, 08:59 AM
By steeplejack in forum Marketplace DiscussionReplies: 3Last Post: 19-10-2013, 09:52 PM
By stewpid22 in forum Projects, Jobs & RequestsReplies: 0Last Post: 21-09-2012, 12:11 PM
By kylelnsn in forum Items WantedReplies: 5Last Post: 09-08-2012, 08:54 PM