Printable View
Hi All
I am new to this forum and would like to start out with a question about cooling.
I want to mill 12 mm aluminium on a pretty basic mill, 600w spindle 12.000 rpm and a trasition speed of 500 mm/min.
Do I need cooling for the tools? What tools are the best (affordable too) for this type of manufacturing.
Kind Regards
Tonny
Parrafin or WD40 if its just small jobs,
Peter
Hi TonnyQuote:
Originally Posted by Tonny
Sounds rather like you are planning to cut 12mm deep through aluminium with a router at 8mm/s. I can't begin to tell you how much is wrong with that.
Perhaps we need a bit more info
Robin
Power(kW) = KQ/1000, where K = cutting power per cc (17 for ali), Q = volume removal rate....assume 70% efficiency in spindle, 0.7 * 0.6 * 1000 = 17 x Q => Q= 24cc/min, add safety factor of 50% then in reality you'll get somewhere around 12cc/min at a typical feed rate of 0.25mm/tooth.
0.25mm/tooth on a 2 flute cutter at 10000rpm (spindle speed drops under load) = 0.25 * 2 *10000 = 5000mm/min, thats your target feed speed to avoid overheating tool by rubbing, but in reality you'll struggle to acheive that so a comprise will be needed - lets say you can do 500mm/min....
12cc = 1200mm3/min, if the cutter is endmilling 3mm wide at 500mm/min then the depth of cut = 1200/(3 x 500) = 0.8mm
for 12mm thick ali you'll need 15 passes for the depth, times however many for width...
a larger dia cutter you'll need to reduce the depth of cut proportionally, or risk burning out motor/stalling it/breaking cutter or usually all 3... larger cutters will need a slower spindle speed... if you can vary it...
however start with a lower feed rate... increase DOC from .2mm until machine complains (and it will) then back off 25% - you'll soon learn limits of machine and cutter (and you'll break a few so get some in)
Is there anything you dont now Irving? :toot:
The only advice I can can give is to get the right cutter. I started using some old end mills that I got as job lot, good condition and sharp, but the results were poor, 1mm DOC and the sides had burrs.
Then I got the Alumex??? ,or some thing like that, especialy for Ali (different helix I think) and the difference was really noticeable, sharp edges and 3mm DOC. I've now got flex issues with the machine to sort out. but thats another story :whistling:
Note. my spindle speed and feedrate were a lot lower than yours, dont now any figures just that it worked.
Irving is right, basically relatively light cuts repeated, 0.8 sounds about right, you could rough it first by plunge drilling? The cutting speed should be about 100m per min, by that I mean the speed of the tip of the cutter against the job. So feed will vary depending on spindle speed and feed rate. It can be cut very fast but you will need, serious cooling. The problem with ali is that if your feed too slow, the ali work hardens and gets hot, if too fast it gets very hot, you get a sort of micro melting at the tip of the tool, the ali will stick to the cutter, bind it and eventually you will find you're just melting through! With experience you will be able to here what your machine is saying to you. Have a look at the tool, is their ali on it? Less feed or more coolant (parafin or water). if you've got a nice coolant tray then you cant give it enough. If you havent you can do it manually with a brush, WD40 works fine (to cool) but is a lubricant, not cutting fluid, cutting pastes work like trefolex (washing up liquid) and stay in teh groove but will only work if you keep the feeds and speeds down. If the job heats up, takes a lot of cooling. When you see the type of high speed deep roughing of ali on youtube etc, note the very ample application of coolant. Quick bit of mental maths at 100m/min tip speed with a 3mm cutter and Mr Irving is within a nats whatsit. If you can cool it well then you can drive up the feed a bit (t/c 2 flute!) but not too much. Inspect the tool, is the ali melting and depositing on the tool, thats your indicator. Hope this is of help. Tom
Paraffin is the "preferred" coolant for aluminium.
Feeds / speeds: not sure quite what kind of work you're trying to do, (pockets, profiles, holes, facing, or indeed the size of job) - machine rigidity and workholding set-up will affect the feed and speed you can apply. I've always managed with standard HSS slot drills / end mills (but good sharp ones, preferably new), though I've no doubt Aluminium-specific tooling would be better (I only do ali on an occasional basis, and generally use my own judgments). The surface finish required (is it specific?) will also affect speeds and feeds you can use.
Some more info would be useful.