Any tips for deep slots/profiling in aluminium?

I'm looking at milling some parts from 6082 Aluminium, however they involve 2mm radius corners and 8mm depth, so I'm looking at 2x cut depth to diameter ratio, if I go for a single slot.

In steel this wouldn't bother me, as I'd just use a bit occasional WD40 application combined with yhe occasional blast with the airline to keep as much of the swarf out the cut zone, however I know this technique doesn't work well when dealing with aluminium that prefers to stick to cutter edges for the slightest reason and start a terminal spiral for cutter life.

My current thinking is use a 5mm cutter to do a rough profile (I'm using a 5mm as it's the best compromise for a few surface features I need to do first), leaving 0.1, and maybe 0.5mm depth, then swap to a 4mm cutter for a couple finishing passes, with the last being at full depth.

I know the best option is flood coolant, however it's not an option on this mill.

So any hints/tips from anybody who's dealt with deep slots in aluminium without flood coolant?

I don't usually do deep slots that deep single pass unless using a ripper and even then I'd be very weary with small cutters.! . . .(That thou is mostly down to low torque high speed spindle)

I find air blast and air mist is the best option for cutting aluminium. Unless flood is high pressure and lots of it then it's not as affective at clearing chips so you don't get as good a finish in Ali.
In your case if you can't do the mist I'd just have a constant air stream clearing chips and keep giving odd squirt of WD.

I don't know about aluminium but with wood an upspiral bit would help clear the chips, unlike wood the aluminium is not going to splinter on the top surface by using it. I would definitely use a larger cutter for the roughing cut as you say.

Quote:

---

Originally Posted by EddyCurrent

I don't know about aluminium but with wood an upspiral bit would help clear the chips, unlike wood the aluminium is not going to splinter on the top surface by using it. I would definitely use a larger cutter for the roughing cut as you say.

---

Eddy Milling cutters all tend to be spiral flute it's just the Helix angle that changes.

Yes but without researching it I didn't know if they were up or down spirals or both ?

Quote:

---

Originally Posted by EddyCurrent

Yes but I didn't know if they were up or down spirals or both ?

---

Well technicly it's possible but you buy Left handed flute tooling and run the spindle in reverse which as the same affect as down cutting or for special cutting conditions where only one direction can be used that would say normally only allow conventional cutting but you want climb mill finish.! or vise versa.
The norm tends to be mostly up cutting with milling tools as like you say breakout is not a problem and everything is usually clamped down tight. You can get them for Composite materials like Carbon fibre and they do Unequal Helix and rougher/finish in one tool etc but they tend to be expensive and often PCD tooling(diamonds). But for general milling and Aluminium then mostly just right handed spiral flute with helix angle to suit material.

I think M_C your biggest problem will be spindle speed with small tooling as most mills don't spin fast enough for smaller tooling and Deep.

Looking in my Cutwell catalogue the spindle speed for 3 flute 5mm HSSE coated Slot mill is 8200rpm and 610mm/min but with only 0.5 x D.
2 flute would be 6300 and 310mm/min same 0.5 x D

Going to uncoated Carbide 2 flute would be 6400rpm and 320mm/min but with 1 x D.

3 flute rippers will let you go 1.5 x D but they still need high rpm and I can only see them at 6mm no less. I use Carbide rippers all the time and they shift some material even with my WC 2.2Kw spindle so if you could get away with usinfg 6mm they would do the job.

I've already ran the various figures through FSWizard, and know that spindle speed is the limiting factor, so I'm really looking for coping strategies.
I'll try single slotting it first, then if that's going to cause issues, I'll try and figure out some way to do a wider/double pass slot to create swarf clearance/make clearing swarf out easier, however that might involve lots of code fiddling in CamBam :/

My last attempt at cutting something out of 8mm plate resulted in the 4mm cutter getting destroyed at about 6mm depth.

This is a kind of exploration for a possible new product, so I'm looking to make it as pain free as possible on my existing little mill, and depending on success/failure will decide on my next machine.

Full depth trocoidal milling is probably best with a 3mm ripper, drill for the entry and stepping over .3mm on the passes. Then finish the last .1 with a single pass.
I'd use a 3mm ripper from WNT (I have no financial interest in the company), the 2 flute 50 960 030 would give you plenty of chip evacuation whilst still keeping up a decent feed and has about 12mm of cutting lenght.
I don't know your spindle limitations so I can't call the speeds and feeds. Just watch the corners, obviously one wrong move and snap but if you have a cad/cam system and if it is for a possible new product you can prove it with a 1mm DOC. A bit of planning would save you lots of time down the line.
Best of luck with it.
Noel.

Thanks for that, I knew that circular milling technique had a proper name, but my google-fu wasn't strong enough to find it!
Just had a quick search over on the CamBam forum, and it can apparently do itm so I'll go and do some reading and try it out.

I had a first attempt today, and it went pretty well. A continual gentle stream of air, combined with the odd squirt of WD40 kept things running well using the 5mm cutter to do the main roughing profile pass using a pretty conservative DOC. I never got to the 4mm stage, as I screwed up the toolpath generation meaning it bypassed spiralling a couple key holes in the centre, so I never let it go any further.