CNCEST 6040 Newby problem with milling aluminium

Hello,

I got a 6040 China CNC and I wanted to mill some aluminium with it. I am completly new to CAM and CNC so I Used Fusion 360 to create the model and the CAM Module from Fusion 360 to create the G-Code for Mach3.
I have used a Carbide 6mm bit with 2 flutes as I was told that is best suited to mill aluminium.
And I have used those settings in the CAM module to mill. Cut feed rate is 100mm/min. Plunge and Ramp feed rate is 30mm/min and Lead in/out feed rate is 50mm/min. I mill in several passes with 0.1mm depths each and the spindle is set to 10000rpm.
The problem that I have is that in the last pass when the bit cuts thru the bottom of the part, the bit catches the thin rest with the flutes and then it grabs the workpice.

The bit then cuts chuncks out until it breaks.

I guess I am doing something wrong, but have no idea where to start.

It looks like your part needs to be fixed to the table. Screws at the 4 corners and in the center island would be helpful. Also you need to use some cutting fluid, WD40 works well for aluminum.

That is not a milling machine. It's not ridged enough. Carbide cutters will chip and brake with the vibrations that are generated. You might try HSS cutters but rigidity will still be a problem. Milling a internal parts needs to be held down that is why it is lifting. Once you have those holes milled out fashion a couple of wooden toe clamps to hold it down for the outside cuts. That is how I do it.
Jack

I have used a cooling fluid when I did the milling, here is a video from the milling:

https://youtu.be/jSFOleQ78ZI

I already thought that the T-Nut table would be too flimpsy as there is no support over the whole depth. And it is made of 120x16mm extrusion profiles, instead of a whole plate. So I noticed already that those bend when you clamp something down. Also those cheap hollow extrusion profiles bended when I clamped it down with too much force.

So I ordered a 10mm steel plate to mount on as the table and got a cut off leftover from a massive T-Nut table made from 250x20mm profiles to mount on top of it. I plan now to drill the M3 holes for the profiles with a 3.3mm bit and cut M4 threads. Then I plan to use countersunk M4 screws to bolt it to the frame. The massive T-Nut profil will be bolted to the steel plate then.
That should bring the requirred rigidity to the table. Even when I lose some height on the Z axis. If that works well I may cover the whole table area with the new T-Nut profiles bolted to the stell plate.

But I have seen video that people mill even 1/2 inch aluminum plates with those cheap CNC routers. I was wondering how I can tune the milling parameters.

It looks like you are doing it correctly. The steel plate will be a lot of help, it will give you something solid to attach the parts to. When using flood coolant, I use an aluminum spoil board and screw the parts directly down to the aluminum. When using mist coolant, I use MDF for a spoil board.

I'd be using machining tabs and a spoil board for this, as well as mist coolant or just the occasional squirt of WD-40.

Your feed rates seem super slow, too, for a carbide bit in ali. My carbide 6mm two flutes run at 18,000 rpm, 300mm/min ramp feed rate, 2000mm/min cutting rate and I've given up on shallow cuts in favour of deep adaptive milling. Uses much more of the cutter, goes much faster, tools last longer blah blah blah.

So, for me (and others may have their own way of doing things):
- sketch in some tabs, say about 6mm wide, 0.5mm - 1.0mm high, 10mm long every 30mm or so around the perimeter. These will hold your part in the workpiece even through the finishing cut, then just knock 'em out using a coping saw.
- use an adaptive strategy to do the profile with a work envelope of the silhouette offset by 8mm to give the cutter room to breathe. Exclude the tab sides from the operation.
- Helix in, go full depth and use an optimum load (radial width of cut) of 0.8mm or so on your cutter with a radial stock to leave of 0.15mm or so.
- Add a profile operation as a rest operation to knock that last bit off and finish the edge.
- mount it up on a spoil board. Bit of flat but scrap ali sheet, bit of plastic, I often use old HDF floating floorboard offcuts even.
- crank up your feed rates. Use a feed/speed calculator to work out what your optimum is then scale it all back (feeds and spindle rpm) based on what your machine can/can't do. Might be worth just having a play with a few bore holes in the scrap you have in the photos to see what good feed rates are for the ramp and main operations.
- lubricate your cutter (methylated spirits 20% in water mist or wd-40 squirts both work well, the metho leaves the machine lots cleaner) to prevent edge welding and, if you can, air blast it to clear chips. Recutting chips is bad for the tool.
- have at it!

Do you have specific machine set up in Fusion 360 that you use for your machine?