First cut in aluminium. Disaster.

[Edward]

Well, since I originally posted, I've been learning a bit about my mill and no more endmills have been broken.

I now use the Alu-power carbide 2 flute and 3 flutes from Cutwel. They are a little more expensive but they work well. I know it's overkill but I like good quality sharp and shiny tools :)

My mill can only do 2000revs. which I always use.

Using Fusion360 with Adaptive to cut a pocket or remove material I use an 8mm 3 flute cutter, Helix plunge down fairly slowly (20degree angle) to about 6mm depth with a plunge feed of 300 and WOC of 0.5mm. Once it reaches the 6mm depth, I go faster at 350 feed and 0.5mm to enlarge the pocket. Then repeat the same with the next 6mm depth and so on.

I use no coolant or air, just a vacuum to suck the swarf. No problems at all at these settings.

It's fairly conservative, I am sure I could go deeper at these settings.

I have tried more WOC, up to 1mm, but that's when the problems start. The TTS type tools can start pulling out of the collet with the consequent accident to follow.

I am sure that if I just used a normal R8 collet only, I would be fine with 1mm width cuts, but with an 8mm cutter it seems to be too much force for the collet to grip the TTS tooling properly. It's fine with smaller diameter endmills though.

Edward

[Ukmiller]

2000 is quite slow for alloy but if you have no coolant or air then i would say you couldnt go any faster anyway.
Aluminium melts so easily and can break cutters

[Edward]

This video shows it all, fairly slow plunging, then faster feed (350mm/m) when it reaches its depth. 6mm tool at 2000revs. Using adaptive, leaving 0.2mm to the sides, then finally Contour to finish off to size. Then a tool change to a chamfer tool. This was a test for small ball bearings holes. They fitted to perfection.




Edward

[Ukmiller]

That shows how you machining very clearly.
I would get sacked if i machined that slow though!
But we have 6000rpm and coolant blasting.
Can i ask why you cut clockwise?
I always cut holes anticlockwise to reduce chatter.
Try running the same program the other way to see if it improves the finish you get.

[magicniner]

I would get sacked if i machined that slow though!

Surely if you had good reason no one could argue

But we have 6000rpm and coolant blasting.

And having 3 times the spindle speed would seem to be a contributory factor in allowing you to cut faster?

[Edward]

That shows how you machining very clearly.
I would get sacked if i machined that slow though!
But we have 6000rpm and coolant blasting.
Can i ask why you cut clockwise?
I always cut holes anticlockwise to reduce chatter.
Try running the same program the other way to see if it improves the finish you get.

I think I machine at the speed that my machine allows me to, give or take. I could use coolant or air, but I am happy to compromise and go slower without it.

Regarding climb or conventional milling, as you can see in the video if you have the patience, or fast forward, as I know these videos can be boring, I do the Adaptive clearing in Fusion360 using conventional milling and then as a finish pass I do a last pass (Contour in Fusion360) using climb milling removing the last 0.2mm. This gives me a perfectly shiny and smooth finish, in fact, as good as what I get from any professional workshop.

Regarding the alloy, I normally use 6082T6 which seems to machine fine to me.

So I am happy with a general feed speed of around 350mm/min. WOC around 0.5mm at 2000revs. If and when I have the need for faster speeds, I will build myself a nice router and I will study the good advice that this forum contains. Or I will convert a larger mill. I think for the moment I have a nice little mill that is sturdier than many a cheap router, and does what is supposed to do quite nicely, albeit relatively slowly.

Yes, I broke about 4 endmills at the start, but now things seem to have settled down and if something breaks, it's usually my fault.

Edward