MACHINING 6063 ALUMINUM EXTRUSIONS

I have been trying to machine these extrusions for awhile now with no success. I work at a door manufacturing company and we recently purchased a CNC machine. The extrusions can be anywhere between 30"-96" in length and typically 1"-6" in width/height depending on the piece. Throw in some dove tails and these are a nightmare to machine if you are new to this. I have been using a single "O" flute endmill for a lot of the machining and then a double flute pocket endmill for the pockets. Both are 3/8" and that is all I really have access to at this time. I don't have to make any arbitrary shapes or anything just simple holes, squares and rectangles so our prep devices can fit inside of the extrusion. I can machine most of what I need but I am not getting nearly enough tool life. I have broken both bits quite a few times now. The "O" endmill leaves a nice finish and the harmonics are not bad. The pocket em leaves chips embedded into the finished piece but the harmonics sound fine. Both endmills are carbide. I am at a loss.

I run the "O" EM at:

16,500 RPM's
10 IPM
5 down feed

Double flute pocket EM at:

18,000 RPM;s
15 IPM
5 down feed

Thank you,

You don't mention any coolant/lubricant. Required when cutting aluminum to keep the aluminum from welding to the tool bit. Also your feed seems a bit light for the spindle RPM. Somewhere around 30 IPM or more would be in the ballpark for the single flute, about double that for the 2 flute.

Sorry first time posting on here.

Yes I have a pump attached to the spindle that shoots oil onto the tool. Highest I went was about 28 IPM for the single flute and it chattered the entire time. Damn thing sounded like it was about to take off into orbit. I shall try again.

If you are getting chatter, increasing the feed would be helpful if the machine is robust enough. Full width slotting should be fed a bit slower than more open cutting. Maybe reducing the depth of cut would be helpful. Adding an air nozzle to the system might be helpful to clear the chips out of the cut area.

It doesn't sound like your current setup and work holding are rigid enough. Also coolant is required. I never run a 10mm bit at rpm that high on alloy.

Perhaps try a 1/4" 2 flute bit at those feeds? And add a good heavy vice to stop your alloy shaking and dancing

Sent from my SM-N970F using Tapatalk

Quote:

---

Originally Posted by Jim Dawson

If you are getting chatter, increasing the feed would be helpful if the machine is robust enough. Full width slotting should be fed a bit slower than more open cutting. Maybe reducing the depth of cut would be helpful. Adding an air nozzle to the system might be helpful to clear the chips out of the cut area.

---

I don't think the machine has the rigidity it needs to properly cut that way. It is a 4th axis table that has hydraulic clamps so I can't add my own vice. Would slowing down the spindle speed and increasing the feed rate work better?

Quote:

---

Originally Posted by shanecooney

I don't think the machine has the rigidity it needs to properly cut that way. It is a 4th axis table that has hydraulic clamps so I can't add my own vice. Would slowing down the spindle speed and increasing the feed rate work better?

---

Maybe, the idea is to increase the tooth load a bit. A bit more information about your machine would be helpful.

I have also found that high helix 3 flute endmills designed for aluminum cutting work pretty well. We typically cut 6061 at 6000 RPM (our spindle max limit) and around 80-120 IPM using a 3 flute endmill and flood coolant.

Unfortunately this is all I can really find on the web about my specific machine. Italian made...

https://pdf.directindustry.com/pdf/a...171378-_3.html

I guess this is more of a routing machine instead of a milling machine. Which is why our spindle goes so high. The guy who came to set-up/train started at 18,000 RPM's so I didnt think anything of it until i started breaking bits.

That machine should work. 18,000 RPM should be OK in 6063 with enough coolant, proper cutters, and cutting strategy. You need to bring the feed up to maintain at least a 0.001'' tooth load, more would be better, maybe in the range of 0.005'' if the machine will take it. @18,000 RPM, the feed speed should be in the range of about 120 IPM with a 3 flute cutter, this would give a tooth load of 0.0022'' and a FPM of 1750.

Having said that, plunging in and trying to cut a full width slot in gummy material (6063) is a bit problematic. You don't say how deep you are cutting. In a full width slot you may only be able to go 0.5 diameters deep and need to make two or more passes. If the slot is wider than the tool, then a tricodial or spiral cutting path would work well and then a full depth cleanup pass of 0.01'' or so.

What CAM program are you using to generate the G code?

Thank you, I feel better about the whole situation now. I keep upping the feed rate and it seems to be working a lot smoother. I have been using a helicoidal cut and taking it in 3 passes. The problem I have is the face I need to cut is 1/2" below the top of the piece. I have a picture that will show you what I mean but I cannot seem to add it here.

I use HICAM 3

Trying to add the pic here

Sound like you have it under control. :)