Problems Milling Aluminum M3

[fredz]

Assembled a M3 recently and we are having problems milling 6061 Aluminum.
The job is roughly 30 minutes and is a 3-D pocket clear (Autodesk Fusion 360) in the shape of a U intended to fit over copper pipping.  *see attached picture*
The job seems fine for roughly 10 minutes and then it goes haywire, with heavy banging, router ends up far from the piece, milling into the bed, moving the work piece slightly in the clamps

Using Dewalt DWP611, default 1/4" Carbide Endmill, Rigidity kit, Lowest RPM (16000rpm) setting, 500mm/m feed rate, 200mm/m plunge, 200mm/m ramp, 0.1mm depth of cut, no coolant, 6.0 HP shop vacuum for clearing chips, aluminum lubricant every 1mm of cut (pausing and turning off the mill in between each application)

Additional info: There seems to be a bit of concerning vibration when the end mill is cutting certain directions (particularly 3 o clock to 11 o clock).  We thought it might be the end mill is not level with the bed and tried adjusting which seems to lessen it slightly or change the direction when the loud vibration is occurring.  

Things we tried:  Tightening all the belts, Making sure V-wheels have no give, Making sure there's no backlash, Trying to level everything.  Cuts seem to be perfectly fine with wood.

Attachments:

[Derek the Admin]

I bet it’s gumming up on the ramp. Does it seem like a ramp move is where the problem lies? Feeding too slow can create problems. Also, it looks like you are slotting. Have you thought about using a 1/8 end mill to do an adaptive clear then cleaning up with a pocket op?

[fredz]

Hey Derek,
Not sure if the ramp move is where the problem lies because it works fine for around 10 minutes of running. If feeding too slow can create problems what should the recommended specs be? We don't have an 1/8 end mill but we might do the adaptive clear if increasing the feed rate doesn't work.

[Derek the Admin]

It's probably having chip clearance issues or gumming up from heat then. If the end mill is dull (if you've had failed attempts its likely grown dull) it will be hard on the machine as well.

I'd go with 800mm/min feed, 0.15mm stepdown. I'd ramp at 700mm/min and plunge at 350mm/min. I would recommend going adaptive. Your toolpath involves slotting, which is hard on any machine.

[fredz]

Update:
It seems to be juttering quite a lot on the xy movements when we increased the feedrate (visibly jumping up and down)

[fredz]

OK, we'll try changing the bit and using those settings and use adaptive clearing. We'll keep you updated.

[fredz]

Hey Derek,
Thanks for the help it just finished an hour and half job! How aggressive of DOC/Feedrate can we take? (An hour and a half is quite sometime to be waiting)

[Derek the Admin]

Nice work. If you are using the adaptive strategy you could probably go with 0.3mm depending on how much radial cut you are taking with the adaptive strategy.

[fredz]

Should we keep the 800 mm/m feedrate?

[Derek the Admin]

I would. There or a little faster perhaps.