Contour Cutting Aluminium

[Almost Scientific]

Hey All,

Does anyone have recommendations regarding bits, speeds, and feeds for doing 3D contour cutting on some 0.25" 6061? I've got a PRSAlpha with a 2hp spindle.

Cheers

[Brady Watson]

You'll want to take a lot of care with your 3D roughing pass to make sure that you get close enough to the relief and remove more material than if it were wood. I would leave a 0.015" of meat on the relief instead of the default 0.02-0.04" left by the more popular 3D programs on the roughing pass. How close you get and what size(s) you use (may take multiple roughing passes) will determine what size finishing tool(s) - (yes, it may take multiple finishing passes as well) you will need.

As a reminder - you ALWAYS ramp into the cut on the roughing pass with aluminum, brass and other hard materials. NEVER plunge straight down.

Shoot for 13000-15000 RPM and .7-1.2 IPS XY, .4-.7 IPS Z speed. Limit depth of cut to NO GREATER than .06" per pass, with .02-.04" being a more realistic target. A single spiral-O flute tool from Harvey Tool or Onsrud is fine, or get a high speed steel (HSS) 2-flute end mill made for milling AL from ObergBrothers.net - HSS works better with AL than carbide.

-B

[Almost Scientific]

Thanks Bradly,

Based on your response I assume I can use any of the tooling I would use on my Bridgeport to cut AL, so I could contour with a HSS, two-flue 0.25" ball nose endmill, and use the single spiral o-flue for the roughing, yeah? Any particular reason I can use a standard two flute HSS endmill for roughing?

Also, are you speed, feed, and DOC recommendations the same for the roughing and finishing passes?

[Brady Watson]

You can use the same tooling as your mill, although the single spiral-O tools work a bit better on the router since you are reducing the number of part rubs (heat) with a single vs 2-flute. Take care to NEVER plunge straight down - ALWAYS ramp in the XZ or YZ plane into the workpiece while roughing, or come in from the side from dead air space.

A 2-flute ball should handle 3D finishing, but you might want to kick it up to a 4-flute if you find the chipload too heavy on the finishing cut using the 2-flute. Keep the part securely held to minimize vibration and keep the tool and workpiece cool. The part will get heat soaked if not properly cooled.

Every part is different, but start out slow and observe how things are going. You want to avoid crashing and shock loading the tool into the part...and you want to get the tool to move as smoothly as possible since AL is dense - any vibration will telegraph into the finish.

You may want to adjust your VR Slow Corner Speed down to somewhere between 25 and 35 to add some cushion at direction changes. Also, make sure you rough out completely around the perimeter of the part - you don't want the ball crashing into a wall of ambient material every time it gets to the min or max raster extent on each stepover line. Proof the toolpath in scrap if you are in doubt.

-B

[Almost Scientific]

Awesome Thanks!