Aluminium Feed and Speed

I’m moving onto Aluminium now and could do with your advice on the following settings in Easel.inventables. I’m going to test cut a square out of 3mm aluminium, and will subsequently try 6mm, 10mm and 15mm thick aluminium as I have samples available.

I have read these but am still not clear what combination is a good baseline considering Ryans message in Link-1, but my setup is the same as Ryans in size:

  1. Aluminum Guide | V1 Engineering Inc
  2. Milling Basics - V1 Engineering Documentation
  3. https://docs.carbide3d.com/support/supportfiles/S3_feeds_250.jpg
  4. Materials - ShapeOko
    and more…

But I am looking for someone to give me a simple baseline for all the settings to start from for my tests, so I at least don’t end up blowing out my 1/8th inch bit within 1 second of cutting.
Question-1: Could you tell me what settings to use as a baseline for cutting Aluminium (Aluminum for the Yanks), and any further things I should have included in my list below but didn’t?

DoC - 0.5mm?
FeedRate - 10mm/s?
PlungeRate - 0.5mm?
Speed - Makita setting ‘1’ (10K)
Endmill - single flute, upcut, 1/8th inch

Additional info:

MPCNC-Primo dimensions - 3’ x 2’ and 4" z-axis height (but will reduce using stacked planks from Link-1 info)
Router - Makita 700 series
Easel.inventables doesn’t have ‘tracoidial stepover cutting’ or ‘adaptive clearing’ from what I see.

Right now, I have no chip-clearing apparatus but will make do during these tests and buy the gear in.
You suggest ‘Husky 4gal air compressor’ but that’s only available in the USA.

Question-2: Do you know what other air compressor I can get that’s cheap and reasonably quiet on Amazon?

You can also use a shop vac for chip clearing. I don’t know what setting 1 is on a Makita, but with my DeWalt your other setting would be a good start.

I don’t know whether Easel has got Trochoidal Milling, but it’s the go-to tool for the MPCNC. :slight_smile:

"Christian Knüll empfiehlt in Estlcam für Aluminium eine Wirbelzustellung von ca. 2-5% (Richtung 2% für schmierende Legierungen, Richtung 5% für eher unproblematische, harte Alulegierungen)

Tiefenzustellung gerne mit 2-3facher Fräserdurchmesser, allerdings darf nicht zu schnell eingetaucht werden. Beim Vorschub was die Maschine hergibt ohne sich allzu sehr aufzuschaukeln. Drehzahl mittel bis hoch, also im Bereich von ca. 18.000 bis 28.000 U/min." I quoted this from another page, because I can’t find the forum entry any more where he wrote it himself, but it is basically taken 1:1 from there.

I am trying to briefly translate: Trochoidal with 2-5% (2% for very soft materials, 5% for hard ones), DOC 2-3 times the endmills thickness (so 3/8 inch for you), as fast as the machine can go without begining to swing, 18 - 28.000 rpm.

/edit: Found the original post, translator might help: Alu fräsen - Tipps & Tricks - CNC-aus-Holz

This is what I used to cut out my Lowrider plate:

DoC - 0.1mm
FeedRate - 1mm/s
PlungeRate - 1mm/s
Endmill - two flute, upcut, 1/8th inch

1 Like

I would like to piggyback on this question. I recently (yesterday) started my luck with milling Aluminium on MPCNC. I started off with trochoidal and I got decent sized chips (beginner’s luck) with the following settings in ESTLCAM:
Endmill: 2.5 mm, single flute, upcut
Depth per pass: 3 mm
F(x,y): 20 mm/s
F(z): 5 mm/s
Stepover: 45%
Trochoidal stepover: 10%
Trochoidal width: 50%
I sacrificed 2 endmills to get to the above settings but the cuts are consistent now.
The problem I am running into is when I use regular milling. Here are the settings that I used based on the metal milling article:
Depth per pass: 3 mm
F(x,y): 5 mm/s
F(z): 5 mm/s
Stepover: 45%
The endmill gummed up and broke. I do use an air blast for chip clearing. Was I being too aggressive? @kcny settings above appear very different. I am inclined to try and experiment with different settings but isn’t the above too slow? My current strategy is to start with these settings, then increase the feed rate till I hit 20 mm/sec and then increase the DOC. Is there a better strategy?

Did you gum up during the cut or when entering it? Changing the ramp angle can help a ton, instead of plunging straight in you can have it ramp down along the tool path to prevent clogging the flutes on the start.

5mm/s is a little on the slow side where you may be rubbing more than cutting, but that also depends on the rpm of your spindle and your cutter material. Can use a calculator like FSWizard to figure out a starting point, the feed per tooth (Fz) should be .001" or .0254mm as a minimum starting point.

Thanks Alex. I did some more experiments today. The following settings work fine. May be I was too aggressive with DOC earlier. I will try to fine tune further like the ramp angle.
Depth per pass: 0.5 mm
F(x,y): 10 mm/s
F(z): 5 mm/s

It’s a tough thing to dial in, every machine is different and all cutters aren’t created equal. 1/2 the tool diameter has been my starting point for DOC, maybe 3mm was too much, maybe the path you had didn’t let it clear the chips, maybe you were going too slow and just rubbed the tool until the aluminum galled up on the cutter.

In F360 I have been using a 2~5 degree ramp in for aluminum, might be a good starting point for you, might not be since I run 2 flute cutters.