Question Aluminium settings

Hi guys,

I had my first attempt at Milling aluminium, with disasterous results. The Bit chattered, lifted and then jammed the spindle. I was using recommended speeds and feeds for roughing aluminium, with .0035 Chip loading, and tried recommended cut depths - although there really aren't and " recommended " cut depths for aluminium.

I can see a lot of guys using 0.2 to 0.3 mm cut depths on a 3mm bit, which is nothing like the 1/2 diameter Rule of thumb. How are guys coming up with these numbers? - are there any tables that actually talk about cut depth. The Wizard calculator was even telling me 1.5 to 2mm roughing, which also did not work?

finch wrote: I had my first attempt at Milling aluminium, with disasterous results....

We're talking about aluminum or about aluminum ....
Note: If you don't know the metal alloy, everything will end up in a trial/error/success event.

finch wrote: ... are there any tables that actually talk about cut depth.

This is not much but it gives you an first idea.
Note: "Zustellung" in German means "cut depth":
cnc-wiki / Parameter Metal

I don't know a lot about metals but from what I've read, aluminum has lots of variants/alloys.

While one can be soft to machine like plastic, other can be hard as steel.

I suppose you got one of the hard variants.

Check this wikipedia article: https://en.wikipedia.org/wiki/Aluminium_alloy

And this shapeoko wiki list: http://www.shapeoko.com/wiki/index.php/Materials#Aluminium

hi.
please ask me.
i will give all the information u need
This email address is being protected from spambots. You need JavaScript enabled to view it.

Hi,

So I did some basic testing on unknown aluminium, starting with varying RPM, then cut depth, and havn't gotten to varying feed rates, but that will be next. 6mm end mill Carbide 4 flute upcut.
3,000 RPM 150mm/min 0.1mm Depth Ok Cut silent
5,000 RPM 150mm/min 0.2mm Depth Ok Cut Slightly vibrational noise
10,000 rpm 150mm/min 0.2mm Depth Ok Cut Less vibrational noise
20,000 rpm 150mm/min 0.2mm Depth Ok Cut silent..... 20,000 rpm produced the quietest and "easiest" cut.

20,000 rpm 150mm/min 0.5mm Depth Ok Some Cut noise
20,000 rpm 100mm/min 1.0mm Depth Ok More Cut noise + Vibration noise
-Cut 1. Suspect poorly bolted down work piece caused chatter + path wander and jam.
-Cut 2. Piece now secured firmly, cut ok, " normal noise + small vibration from loose Z axis to X AXIS MOUNT
-Cut 3. Piece secured firmly, however still small play in X axis mount, causing small occasional vibration
20,000 rpm 100mm/min 2.0mm Depth Cut noise, workpiece vibration + play in mount cause wobble and Jam - cut terminated

The workpieces and end mill temperature were checked immediately following the cut, and both were cold to the touch.
The HF spindel motor was warm/hot to the touch

At the moment - the rigidity of the machine seems to be the big limiting factor. I think 2mm with the x/z mounts tightened shouldn't be an issue.

Will update this after more testing.
Nick

Hi,

finch wrote: I can see a lot of guys using 0.2 to 0.3 mm cut depths on a 3mm bit, which is nothing like the 1/2 diameter Rule of thumb. How are guys coming up with these numbers? - are there any tables that actually talk about cut depth. The Wizard calculator was even telling me 1.5 to 2mm roughing, which also did not work?

Most tables and calculators are for heavy industrial machines.

• The cutting forces for aluminum are high - so depth per cut needs to be very low on light machines to avoid vibrations and tool deflection.
• Another problem is that aluminum tends to stick to the tool as soon as the tool gets too hot. To avoid this the chip needs to be rather thick - meaning low rpm but high feedrate. This combination of low rpm and high feedrate is often hard to obtain with fast running spindles.
• Generally:
  • Use low depth per cut.
  • Try slow spindle speeds - but keep feedrate rather high.
  • Use some coolant - aluminum cutting oil or even vegetable oil will improve results alot.
  • The harder the aluminum the easier to machine. Soft aluminum alloys typically used for anodized profiles are the worst. Aluminum alloys with lead like AlMgCuPb are easy to machine.

Christian

Maybe there is some useful information on the following CNC Cookbook links:
link 1
link 2
You might have to fight some advertising banners when opening those liks.

You could also browse some cutting tool manufacturer datasheets for comparison. For example Mitsubishi Materials, Sandvik etc. Maybe that would give some indication what a 6mm Carbide 4 flute upcut end mill needs when cutting aluminum.

REVISED RESULTS - MORE DATA

6mm end mill Carbide 4 flute upcut.
3,000 RPM 150mm/min 0.1mm Depth Ok Cut silent
5,000 RPM 150mm/min 0.2mm Depth Ok Cut Slightly vibrational noise
10,000 rpm 150mm/min 0.2mm Depth Ok Cut Less vibrational noise
20,000 rpm 150mm/min 0.2mm Depth Ok Cut silent..... 20,000 rpm produced the quietest and "easiest" cut.

20,000 rpm 150mm/min 0.5mm Depth Ok Some Cut noise
20,000 rpm 100mm/min 1.0mm Depth Ok More Cut noise + Vibration noise
20,000 rpm 100mm/min 2.0mm Depth Cut noise, workpiece vibration + play in mount cause wobble and Jam - cut terminated
Z Axis + X Axis Mounts tightened, and feed rates tested
20,000 rpm 100mm/min 1.0mm Depth
20,000 rpm 200mm/min 1.0mm Depth
20,000 rpm 300mm/min 1.0mm Depth
20,000 rpm 500mm/min 1.0mm Depth
20,000 rpm 600mm/min 1.0mm Depth
20,000 rpm 650mm/min 1.0mm Depth All Cuts up to this point, sounded and appeared the same, Noisy with minimal vibration
20,000 rpm 750mm/min 1.0mm Depth Cut started, then stopped by itself and it was evident Y axis had lost position.

Next Test, will be to select a feed rate around 500, and reduce RPM to suit chip load, and see if the machine copes with the slower RPM ok

Christian Knüll wrote: The harder the aluminum the easier to machine. Soft aluminum alloys typically used for anodized profiles are the worst. Aluminum alloys with lead like AlMgCuPb are easy to machine.[/li]
Christian

Wow! I'm using 6060 aluminum 'cause I was sure it is the easiest to machine...
Are you sure that AlMgCuPb is better?
It would be the one noted as "1060" in wikipedia , I'm right?

Hi,

julius wrote: Are you sure that AlMgCuPb is better?
It would be the one noted as "1060" in wikipedia , I'm right?

AlMgCuPb is equal to EN AW-2007 (not in the Wikipedia list) and contains up to 1.5% lead - much more than EN AW-1060.
This alloy is really easy to machine and quite strong - but also very brittle (you can't bend it - it will break).

Christian

Hallo Christian, danke for your reply.

About Aluminium EN AW-2007 I read:

Precautions and Warnings: Poor resistance to atmospheric corrosion. Hard anodizing or other protection is recommended.

So, just for speaking and bubling, it's not the perfect material for an application like mine (an instrument mounted on a motorcycle). Whereas the Alu 6060 has a very good resistance to corrosion.
The EN AW-2007 can be painted like the 6060? The paint will solve this corrosion problems? (I don't know if you can answer to my specific questions.)

Hi,

painting aluminum is very difficult and not very common.

The main problem with materials like aluminum is availability. Alloy lists like those on wikipedia are nice - but in reality there are less than 10 alloys you can actually buy without ordering a whole truckload. So instead of searching for the perfect alloy you need to see what you can get and then select the least troublesome. As with almost everything good properties in one aspect usually come with bad properties in others:

• AlMgCuPb is just heavily optimized for machining with large tradeoffs for anodizing, welding, bending and corrosion. This is one of the very few alloys where you can be far off optimal tool and cutting conditions yet still get good results.
• The opposite are AlSi alloys. They are made for extrusion and anodizing. They can be machined, too - but with very little margin for errors.
• AlMg alloys are very common and have medium machinability and good corrosion resistance. They are sometimes offered with different hardness - the harder the better to machine, the softer the better to bend.
• Another 2 common alloys with good machinability and corrosion resistance are AlZnMgCu1.5 and AlMg4.5Mn.

Christian

Thanks Christian, you're a huge source of info!

BTW. I've found just now a web site that can be useful for everybody (I hope):
AluSelect

(You can select "Formability, Machinability & weldability" on the left menu and compare the MAA index for different alu alloys. Nice! - 2007 alloy has the highest MAA index, but it's not the only one)

Now I'm wondering a little more, the Y axis has the heaviest load on the entire machine by design, cutting along the X axis would be far more Rigid, and then cutting with the indexed 4th axis, more rigid again, probably allowing much faster ( normal ) rates

finch wrote: Now I'm wondering a little more, the Y axis has the heaviest load on the entire machine by design, cutting along the X axis would be far more Rigid, and then cutting with the indexed 4th axis, more rigid again, probably allowing much faster ( normal ) rates

Your're right.

BTW, I've just ordered a small plate of EN2007 alu (i.e. DIN AlCuMgPb) to make some test. Unfortunately that material cannot be used outdoor, but I think it could be perfect to produce fixtures.

For outdoor application I think that the best compromise is the EN7075 alu (i.e. DIN AlZnMgCu1,5), even if it is not recommended in marine and industrial environment.

In any case 2007 and/or 7075 materials are hard to find, there is no big choice as 6060...
For example, I was searching for a 7075 50x50m square section tube (Quadratrohr) and... no way to find it in Germany.

My little contribution after some tests on a square 50x50mm alu-profile doing 1 or 2 mm deep pockets.
Below the settings that I feel comfortable with:


What above is not a scientific test. I've tested various speeds and feed rate while listening just at my ears.
In other words, above settings give me the "impression" that the machine is working smootly, I cannot say how much is true and how much is pure imagination.
Maybe I could use more aggressive settings but tool deflection problem is always with us.

I have to say that I'm not completely satisfied when doing small cylindrical pocket. By using an helicoidal path I still hear a little "grrr grrr" noise at the start of any down-step. No way to eliminate it completely (suggestions are welcome).

Happy milling!
Tschussssss!

BTW, I was using this end mill .

Uh! I've found a (low quality) photo about milling several pockets with the settings published above (pockets are 1,5mm deep).

This image is hidden for guests.
Please log in or register to see it.

Hey great info you've posted here ... this a nice post which I missed... but found very helpful later. My salutations to everyone on this thread https://stepcraft.us/aluminumspeedfeed/