[R3dplanet]

I've been having some issues milling 6061 aluminum. Nothing major, I think I've figured out the main problems.

I have one general opinion question though. My machine is an industrial machine so it can handle aluminum but what I'm curious about is even though I can run up to 20,000 RPM and been initially testing at 15,000 RPM with 18,000 RPM max bits, should I just run slower for better cuts and less issues?

To note what I've been testing lately is a single flute carbide bit at 15,000 RPM at 60 IPM and .004 chip. I'm not exactly happy about the look of the cut.

I've tried slowing it down but then the aluminum gets to hot, welds, and breaks my bit.
So I tried faster and still the aluminum got too hot and I ended up losing another bit.
(To not this is of course contingent on what type of cut. Using a 2D adaptive in Fusion 360 and chipping away it doesn't have issues really but still not the cleanest cut)


Should I just run Aluminum cuts at say 5k-10k RPM and take on the slower speeds to help reduce heat? I have a built in air+mist cooling system but still seem to be running hot when I run the recommended settings from Amana.


First time Aluminum cutter so any thoughts or advice are appreciated. Thanks.

[ERUS]

I'm going to say the problem is the single flute cutter. Try a 2 or 3 flute with your feeds and speeds. Single flute end-mills are mostly for routers and\or cutting plastic.

[ericks]

I am no expert but i have been using two flute and they work fine....three flute did not work as well as two flute for me. I don't use any cooling, no major heat problems....

[joeavaerage]

Hi,
I use HSMAdviser, I liked it that much I bought it.

https://hsmadvisor.com/.

You have spoken about different spindle rpms, but have not specified the diameter of the tool.

For an uncoated carbide tool in aluminum surface speeds of 200-500 m/min are indicated. At the higher end (500 m/min) you might expect
'built up edge' (BUE) problems without cooling.

For example:

If I use a 3mm endmill:
0.003(diameter in metrers) x PI = 0.09423 m (circumference)
Surface Speed (m /min) =RPM x Circumference
=24000 x 0.09423
=226.1 m/min.
My spindle is maxed out at 24000, so with a small endmill I run it as fast as I can.

If I use a 6mm endmill:
Circumference= 0.006 x PI
=0.01885 m
Surface Speed (at 15000 rpm)=0.01885 x 15000
=282.7 m/min
Note this is comfortably within the 'surface speed window'. I could probably get away without cooling but I get much better results WITH flood cooling so I use it.

If I use a 16mm endmill:
Circumference= 0.016 x PI
=0.0502 m
Surface Speed (at 9000 rpm)=0.0502 x 9000
=452.4 m/min

Note this is near the top end of the window, good cooling will be required. It might be still too high if trying to cut 'sticky aluminium' like the 5000 series
and 6061. If you have problems with BUE then drop the rotational speed to 6000 rpm which will result in a surface speed of 298 m/min. That will help.

Feed rates are simply a matter of working out how many teeth (flutes) are cutting and how much power/torque your spindle has, the strength of the tool,
and if your machine is rigid enough to handle the forces involved.

Lets take my example of a 6mm endmill at 15000 rpm:

At 1% chipload (per tooth), which is conservative, Chip Thickness= 0.01 x 0.006 = 60um
With a four flute tool, Tool Advance Per Rev= 4 x 60um
=240um
=0.00024m
At 15000 rpm, Feed Rate =Tool Advance Per Rev x RPM
=0.00024 x 15000
=3.6 m/min

The important point is that Surface Speed is the main consideration. If you attempt to spin the tool too fast for the material, considering the material of the
tool and whether it is coated or not, you will overheat it. If you turn it more slowly that will be OK but you will have to back off the feed rate as well or you
will overload the tool and snap it.

As a rough guide, for coated carbide tools:
Aluminum 200-500 m/min
Steel 100 m/min
Stainless 60 m/min
Titanium and Nickel Super alloys 25-40 m/min.

These would be roughly halved for HSS tools.

Craig

[Tarzan63]

There really isn’t enough information to make an informed recommendation here. As mentioned above, what diameter cutter? And are you using coolant? What depth of cut? How far is your tool sticking out of the holder?
It shouldn’t matter how many flutes the cutter has. If you get the speed right and are using coolant, and you have a reasonable DOC, then you should have success. Even running without coolant you can do it, at the right speed. If you aren’t running coolant, then no matter what diameter the tool, you will create too much heat at 15-20,000 rpms.