[averageJoe576]

My machine rapids at ~25 IMP, well below the suggested speeds for speed feed/calculation for small end mills.

My spindle can be set to 10,400 RPM. I tried some 1.5mm cutters (4-flute) at max rpm, 20 IPM, 0.5mm cut depth, in 6061 and it worked but the finish was quite poor and the cutters didn't last long (they were quite cheap though)

An suggestions? Do I need to give up on 1.5mm and move up to 3/32"? Do I need to switch to a certain type/style of end-mill?

[CS900]

Well as I'm sure you know, there are a lot of variables that can come into play, but there is absolutely no reason you can't get a good finish within your operating limitations. as far as speeds and feeds go It's all about chip load when it comes down to it. Assuming you are using a carbide tool, you should be well under 20IPM with a 1.5mm EM. Currently you are running around .0005 inches per tooth which is WAY too much for that small an endmill. You should be around .0002 (8ipm). So this also doens't take into account your width of cut, but even if you're slotting at .5mm depth you should be fine so long as your tool isn't stuck out way far.

a couple other random thoughts.
1) using a 3 flute will help your surface finish in AL.
2) HSS tooling will lower your feedrate even more and will work just fine in AL.
3) check the runout on your tool. With a cheap tool I wouldn't be surprised if it's pretty terrible.
3a) make sure your collets are clean
4) coolant! when I had my Taig, I used a spray bottle of WD40. Works great, and you'll be impressed with the difference in surface finish.

[averageJoe576]

Just grabbed some higher quality 3-flute end mills.

WD-40 idea sound great, how often are you spraying? Only for the finishing pass or the whole time?

Also, am I okay to plunge, or do i need to make a starter hole with a bigger end mill?

[CS900]

i spray during roughing and finishing. more so during finishing, but it's not to clear chips out of the way. Recutting chips is a waist of your tool and your surface finish will look terrible as well. I use a mister now that uses compressed air and a tiny amount of cutting fluid to blow the chips out of the way and lubricate the cut. If you have a compressor, they are worth the investment.

You can plunge so long as the tool is center cutting. Preferably you would ramp or helix down into the cut though.

[skrubol]

My machine rapids at ~25 IMP, well below the suggested speeds for speed feed/calculation for small end mills.

My spindle can be set to 10,400 RPM. I tried some 1.5mm cutters (4-flute) at max rpm, 20 IPM, 0.5mm cut depth, in 6061 and it worked but the finish was quite poor and the cutters didn't last long (they were quite cheap though)

An suggestions? Do I need to give up on 1.5mm and move up to 3/32"? Do I need to switch to a certain type/style of end-mill?

I think you may be doing your speeds/feeds wrong. Given the same RPM, smaller endmills will need lower feeds. On those .5mm deep cuts, were those slots? If so, I'm surprised you didn't snap your endmill off. 4-flute endmills run aggressively in aluminum, especially without coolant tend to get clogged up and then break.
The only thing that usually limits how small an endmill you can use is runout of the spindle. A 10k spindle won't get anything done too quickly with micro mills, but if you've got the patience, your feed speed shouldn't be an issue.
If you're in the US, you may find a lot more selection of 1/16" endmills than 1.5mm and they're only a hair bigger. Both Maritool and Lakeshore Carbide have 1/16" end mills for aluminum.

[averageJoe576]

Thanks for the suggestion on Maritool/Lakeshore. I've already bought a 1/16" HTC endmill off ebay but will give those a go if it doesn't work out.

How do you calculate feed rate? The standard formula with suggested values (IPT x FLUTES x RPM, IPT=0.0075 for alum) gives feed rates in the hundreds.

[skrubol]

That formula is right, but the IPT depends on the diameter of the end mill as well as several other factors. As CS900 pointed out, IPT for a mill that size should be in the .0002-.0005" range. Is there any information on the endmill you purchased? One of the things I like about Maritool and LSC is they have speeds/feeds charts for most of their mills. The other main factors are the material being cut (IPT is typically much higher for aluminum than for steel,) and the geometry of the end mill. For instance, Maritool's Aluminum oriented 3-flute mills call out .0016" IPT for 1/8" (halve that for 1/16") endmill, whereas their general purpose 2-flute calls out .0008" for their 1/8". Their 4-Fl ALTiN endmills are not recommended for Al, as 4 flutes tend to clog up when running at optimal feed in aluminum, and altin coating tends to be stickier to aluminum (in general don't cut aluminum with a cutter that has aluminum in the coating.)

[averageJoe576]

This what I got

Where do you find Maritool's IPT recommendations? Is there good reference somewhere? I was sure the actual IPT I needed was smaller but didn't know where to find the info.

[skrubol]

Most of the product pages on Maritool have a CLICK HERE link in the product blurb. These are the non-ferrous specialized endmills I referred to above.
https://www.maritool.com/Cutting-Too...202/index.html
Speeds and feeds are what you're looking for. There's a tab on the site you linked. Their chart shows .0011" for 1/8", so .00055 for 1/16". So 16ish IPM as a starting point. Usually you can go quite a bit lower on the feeds, but with micro endmills there's less wiggle room than with normal end mills. Probably keep it above half the recommended chip load if you can. It's a good idea to play with the speeds and feeds a bit. With something this small and a 10k spindle there's probably not much reason to change the RPM (unless there happens to be vibration or something at that speed,) but you can try reducing the feeds and see how the surface finish changes.
Also, slotting tends to give the worst surface finish, going back with a profile cut on each side can clean things up a lot if you've got room.

[averageJoe576]

Ah, got it. Thanks!