Aluminum on the mini-CNC

Tags: #<Tag:0x00007fa49494cc68>
#1

Aluminum is on the list of officially approved materials for the desktop CNC. Mini CNC Machine - Isel CPM 2018.

However, most metal CNC stuff I’ve seen before uses some sort of coolant and when I asked about it around, it doesn’t seem like it’s a common application and someone even said they were told to “ask a CNC tech about it” (but not during my induction).

I have a small piece to mill off from 5x5cm to 4x4cm, and reduce height by 1cm. My thinking is that if I do very long overpasses so the tool cools down and short height passes each time, I should be fine to use on it?

Making 2 flat plates with a handle to lift one of them up
#2

Forgot to tag @CNCtechs

#3

Yes, aluminium is definitely possible. @Archie has a better experience on it and can give you advices.

Thanks
Federico

3 Likes
#4

@palmada & @Archie > Seems like I have a very similar question related to depth of cuts & speeds on aluminium. Any knowledge to share from you guys?

#5

Hello

Sorry, need to write a full article about doing alu.

But in short.

  1. Head over here; 4mm Diameter 1 Flute Carbide End Mill for Aluminium 22mm Flute Length DLC Coated Associated Production Tools (shop-apt.co.uk)

Pick the tool you want (pass depth, tool dia etc.)

  1. Input feeds and speeds from APT Tool page into Vcarve if not already there. Feeds will be faster than our machine can handle.
    Note the chipload APT’s numbers give, reduce feed and spindle speed to keep this number the same untill you reach something our machine can do. Now run at 70-80% of this chipload.

  2. Pass depth, should be no more than 50% of tool diameter.
    e.g. 4mm tool no more than 2mm per pass.

  3. Run first job at 80% feed override, speed up or slow down based on sound. If its complaining lots, slow it, if its making dust, speed it up etc.

  4. Run any finishing passes at 100 - 110% spindle speed, minimum 20% tool diameter engagement (otherwise will overheat).

Notes;
6080T6 Alu machines the best, the softer you go, the more difficult

Buy lots of tools, you will break some, your working on a knife edge of feeds and speeds.

Vacuum very carefully at the end of the job, alu splinters hurt.

Use a big wasteboard, even better if you face it off to make it super level.

Use very strong clamping, make your own fixtures even! (from ply, dont get carried away its alu)

Hope this helps, please post any results!!

9 Likes
Applying foil to bookcloth?
Applying foil to bookcloth?
#6

Yesterday I had a good run at making two of these:

image

Simple enough, but it used Fusion’s adaptive tool paths with an optimal load of 0.6 and a 6ml end mill. I milled 5 faces, cut it off with the angle grinder, then had kept doing facing steps to get the back flat and the thickness about right. It’s hard to capture but it feels very smooth. I was trying to capture some reflections to reflect (pun mostly not intended) how smooth it feels.

Very happy with how it turn out, and no broken tools or ugly marks so far!

5 Likes
#7

Very nice! What are the dimensions? How accurate did you manage to get that? What bits did you use? What are you going to use that for?

#8

So many questions!

40x40x12mm

For this project I don’t need very accurate dimensions; about ±0.1 to 0.2 mm on the sides, and +0.3 in the thickness.

I used them thangs

Should transfer heat from a peltier on one side of a plywood box to the other!

2 Likes
#9

Hey @Archie ,

Thanks for your post with advice on aluminium! I’ve got a couple of questions:

I’m looking to cnc some alu. plate using a 1mm end mill. The APT website suggests:
RPM 18000
Feed 800

You mentioned in your post that we must reduce the feed and spindle speed to numbers that the makerspace machine can handle. Do you know what the max. values are that the machine can do?

You then mentioned that we run the job at 80% of the chipload shown. How is the chipload reduced to 80%? Do we just continue to adjust the spindle/feed speeds to get the correct value?

Thanks,

#10

Archie knows best, but for what its worth:

The spindle on the mini cnc has 6 speeds, option 4, 19,000rpm is closest to what your target, if I remember correctly. I’d program with the 800mm/min feed rate you mentioned and then, using the sliders in LinuxCNC (I think it’s labelled feed rate) you can slow the feed rate down to 80% of the target, probably even lower. If all sounds and looks to be going well, you can ramp it up.

There are a few other things to consider like the depth of the plate. You might have to do it in multiple passes / step overs.

I’d try to use a big a tool as possible and then change to a smaller one for the smaller details.

I’d be interested to know how you get on :). Best of luck. I think the Mini CNC is one of the coolest in the space.

3 Likes
#11

I’d be sure to calculate the suggested chipload (i.g. https://gdptooling.com/chipload-calc/) and see if your settings are below the recommended value.

1 Like
#12

Thank you both! That’s great advice.

Will give it a shot and will update on progress.

Cheers,