Cutting 2mm aluminium

I’m planning to cut an aluminium panel to house instruments for a light aircraft. The aluminium is 2mm thick and consists of a number of 80mm and 58mm holes for the instruments.
My experience with aluminium in the past is that it needs to be kept clear of chips so that they don’t weld themselves to the cutter so I’m using a mist spray and suction to keep the path clear.
What would be the suggestion of the machine path to cut the holes? I was thinking that an adaptive clearing path to cut a 6mm ring on the inside of the hole to be cut (using a 3mm end mill cutter, multiple depths of 0.2mm).

2020-02-20 16_41_19-Autodesk Fusion 360 (Personal - Not for Commercial Use)

Is this the best way to approach this?

The adaptive approach is a good one, but cut deeper. You don’t want to destroy the bottom 0.2mm of your endmill.
I’d also come back with a full depth finishing pass, so keep a small radial stock to leave.

How deep do you reckon I could go?
Currently (not tried this yet), I’ve set DOC=0.2mm, RPM=24000, Cutting Feed Rate=1200mm/min
I’ve used the feed and speed calculator here as a guide

I wouldn’t recommend going any deeper than that. My X-Carve is pretty tight, and I usually don’t go more then 0.005" DPP/DOC on aluminum (that’s a smidge less than 0.2 mm).

Also, if you do the full-depth finishing pass, make sure you’re only leaving about ~0.05 mm or less radial stock, or you’ll end up binding and snapping that skinny bit.

Cheers, I’ll give it a go.
Do you have much success at milling aluminium?

Are you running adaptive toolpaths or slotting? You should be able to cut much more than that on an X-Carve. If you’re workholding is good (superglue and tape), I can’t see why you wouldn’t be able to cut the full 2mm with a good adaptive toolpath.
I was going 3.5mm in this post, and that’s on a Carvey.

Climb or Conventional?

Just take a smaller WOC or optimal load until you feel more comfortable. Faster feed is better, though. That’s where the Carvey is limited.

Here’s an old post with a cut on my Shapeoko, looks like I used conventional…I’d still go with climb if I did it again.

Thanks. I’ll give it a go.

1 Like

I cut aluminum .125" with 500 mm/min, .23mm optimal load at full depth, with an .125 O Flute. I have an x-carve with an upgraded Z axis and a Dewalt 611 router running as slow as possible and run dry.

How do I calculate the optimal load?
How slow is slow on your Dewalt?

16K rpm for a Dewalt 611 on speed 1. The optimal load was from a Winson Moy/Carbide 3D video. He has “cutting recipes” in many of his videos. He had some aggressive adaptive paths after attending an Autodesk conference.

“Slotting” (not adaptive). Considering how small a “bite” that needs to be taken with the X-Carve when using adaptive toolpaths, I’ve never had a project where it would have saved me any time.

The concept behind Adaptive is to go deeper per pass, utilizing more of the actual cutter length.
Thats how you shave off time because you can go deeper per pass.

1 Like

I think most people are leaving some speed on the table with these hobby level machines. I say get that Dewalt off of 1 and crank up the feedrate. The width of cut will be smaller, but going full depth makes a big difference, especially on tool wear. If you pay for an inch of cutter and only use the bottom couple hundredths, you’re leaving that on the table as well.

I appreciate this.

I follow the methodology, but my previous statement meant that I have to keep each pass (even at full depth) so small, laterally (due to the inherent lack of overall rigidity in the X-Carve, and the fragility of the 1/8" bits I’m usually using), that I end up not saving any time compared to doing traditional “pocket clearing” at very shallow depths, but (comparatively) very high feed rates.

1 Like

I found this the other day
This says that Surface Speed for aluminium should be 45 M/M so my toolpath now looks like this (DOC = 2mm, adaptive toolpath)

5000RPM seems very slow to me.

Here is a chart I tend to use myself, my primary target here is feed per tooth
A 3mm tool => 0.025mm/tooth

With Dewalt at #1 (16k RPM)
16.000 * 0.025 * number of flutes => 400mm/min per flute of the tool.
I’d derate the target to 0.020 => 320mm/min per flute and take it from there.

As you can see, the Dewalt will not have the RPM neccesary to take SFM to the max therefore maintaining a target chip thickness is “better” to use.
You could also increase RPM, just maintaining the same chip thickness.
In Fusion set RPM and chip thickness and Fusion do the rest :slight_smile:

1 Like

Thanks. I think I’ll go for this and see what happens

DOC = 2mm or less?

For slotting go easier and increase once a baseline is established.
For pockets use 2D Adaptive and try 2mm first, again increase as seen fit.

I did a test carve once, to find my machine “limit”.
9 equal pockets 25x10mm or so, with depth ranging from 1mm to 9mm.
Feed rate / RPM was equal for all, only DOC was different (1-9mm DOC)
Once the corners started to skew I had my max DOC with that configuration/material.