Cutting aluminum on X2 conversion

[tracebender]

Hey All,

I just completed a CNC conversion of my X2 using the ball screw retrofit kit from CNCFusion. I have it adjusted to the point where I can cut a pretty nice circular pocket in wood using one of the Mach3 wizards but when I try to cut pockets in aluminum I get a lot of vibration.

All I have to work with right now is the twenty piece end mill kit I bought from Harbor Freight. I've tried the 1/4 and 7/16 two flute end mills at various speeds and feeds but seem to get a lot of shaking anytime I plunge, horizontal cuts are better but not what I'd call smooth yet. The box says they are center cutting end mills but I'm certainly no expert in cutting tools.

Any suggestions on feeds, speeds and brands of cutters to use to plunge cut and pocket aluminum on this type of machine would be greatly appreciated.

Thx

[MrWild]

How big of a cut are you making, and how fast are you going?

[H500]

Make sure your gibs are nice and snug.

[TXFred]

If you can avoid plunging, do so. Plunging will put the most force on the X2's weak spot, the column mount.

Try a ramp entry instead. Something like this.

G1 X0 y0 z.1
g1 x1 z0
g1 x0 z-.1
g1 x1 z-.2

and so on. This will move the cutter at an angle down into the workpiece, which should be smoother.

If you have to plunge, play around with the feedrates and reduce it as best you can.

[tracebender]

Thanks for the replies. I believe the gibs are as tight as I can get them without significantly increasing friction. The cuts I was taking were like .050, plunging at 1 or 2 fpm and cutting around 5 or six fpm at around 2000 rpm (my mill won't go much faster.) I tried this with 1/4 and 7/16 end mills (two flute).

It seems that most of my problem was due to the cheap 20 piece end mill kit I bought last year from Harbor Freight. After many disappointing cuts I went to Marshall tool and bought a 1/4 and 1/2 inch end mill made by Melin that are supposedly designed for aluminum cutting; the difference was almost night and day. Any other suggestions on brands, geometry, etc?? I've heard many people prefer two flutes in Aluminum.

Thanks for the suggestion on ramping the cutter into the work. I'll have to experiment with that. Right now I'm just using the wizards in Mach 3 to create the Gcode for the test cuts but I'll try editing some of the code to try this.

[eartaker]

2 flutes work well with aluminum because they don't clog up as easy.

[hoss2006]

The cuts I was taking were like .050, plunging at 1 or 2 fpm and cutting around 5 or six fpm at around 2000 rpm (my mill won't go much faster.)

So you were plunging at 12 -24 Inches Per Minute?
Way too fast, try 5 IPM or less.
We don't use feet per minute much.
A high helix endmill for aluminum will cut much easier too.
And as fred said, ramp when you can.
Hoss

[vlmarshall]

The cuts I was taking were like .050, plunging at 1 or 2 fpm and cutting around 5 or six fpm at around 2000 rpm (my mill won't go much faster.) I tried this with 1/4 and 7/16 end mills (two flute).

Congrats on the successful conversion!

72 ipm at 2000rpm, with a 2 flute endmill is .018" chip load. Slow down your feed, or speed up that spindle.

There are a lot of useful Speed&Feed calculators online, here's one. http://www.dlindustrial.com/Formulas.htm
I've seen a site offering free slide charts like the tool suppliers give out occasionally, if I can find a link I'll paste it here.

[mrcodewiz]

I have found the sweet spot on milling aluminum on my X2 to be about 2IPM in the Z for plunging and between 15 and 25IPM in the X,Y. I keep my DOC under .1 and pretty much stick to 1/4, 3/8 and 5/16 cutters. I think the ones I have now are Niagara aluminum cutting 2 flutes. I also run a 2 groove pulley setup (steele) and put it on the fastest setting and crank it all the way up.

[Teyber12]

those feeds are way to fast... i plunge like 2 IPM in my X3..

its a benchtop mill mate not a VMC you won't be able to take cuts much faster then you did with a manual mill.

[BobWarfield]

It's amazing how much your machining skills improve when you quit using cheap cutters!

Some other thoughts:

- Try a 3 flute endmill. It's like having a 50% faster spindle. I generally buy mine from Maritool. You can even use a 4 flute if there is enough chip clearance, but never in any kind of slot or small pocket. The more flutes, the faster a cutting edge gets to the material at a given spindle speed. That's why I say a 3 flute is like having a faster spindle. But, the more flutes, the less room for chips to get out of the way and the more likely they get jammed with the cutter. I only use a 4 flute in aluminum when it is obvious they can fall out of the way and not build up in a narrow space.

- Get yourself some kind of air blowing on that cut ASAP. Your next issue will be chips packing in. Even just an air blow to keep the chips out helps tremendously. If you have to, stand over it with the nozzle in your hand. That will convince you to build or buy a spindle mounted system ASAP! As you progress, you'll want mist and then finally full flood.

- For plunges, most CAM programs go 1/2 or 1/3 of whatever your regular feed would be for those cutting conditions. HimyKibible recently told me he'd seen a rule of thumb to go at feeds divided by flutes for plunging. I like that rule. However, ramping or helixing is much better. If you get access to a manual machine, try feeling on the handwheels what a ramp feels like versus a plunge. You'll be amazed at how much less pressure it takes.

- By all means, get a speeds and feeds calculator. There are lots of them available. Mine, which is called G-Wizard, is in beta test and is free for the beta test if you want to try it:

http://www.cnccookbook.com/CCGWizard.html

- On the gibs, I run mine almost as tight as I can get them with a screwdriver. This is on an RF-45 and I have pretty powerful servos. If I forget to pump the one shot, one axis or the other (usually Z) will stall at some point in the run. It's really worth it to get them as tight as your machine will stand. There are lots of approaches to adjusting gibs. I think Hoss has published a link to Little Machine Shop about it. Tighter gibs mattered for accuracy and chatter reduction on my machine quite a lot.

Cheers,

BW

[tracebender]

Congrats on the successful conversion!

72 ipm at 2000rpm, with a 2 flute endmill is .018" chip load. Slow down your feed, or speed up that spindle.

There are a lot of useful Speed&Feed calculators online, here's one. http://www.dlindustrial.com/Formulas.htm
I've seen a site offering free slide charts like the tool suppliers give out occasionally, if I can find a link I'll paste it here.

Sorry, it was late, that should have read ipm not fpm.