Machine Aluminum... Spindle speed and flute count

[ngr1]

Hello, can anyone please recommend the appropriate spindle speed (low, medium or high) and end mill to use (2, 3 or 4 flutes) when cutting aluminum.

I have a TAIG CNC configuration and all my feed rates are very conservative (slow) during my testing phase.

Assuming my lube and chip removal is adequate please let me know what has worked for you.

Thanks... Norman

Similar Threads:

• Need Help!- 2.5mm DIA 3 Flute aluminum cutting speed
• require low speed spindle idea for cutting Aluminum
• Spindle that can machine aluminum
• 6-flute endmill for finishing aluminum?
• Tapping aluminum. Spiral flute or not ?

[HuFlungDung]

Norman,

How fast will it go? I bet it won't go fast enough!

Whether you use high speed steel or carbide depends on the practical speed limit of your machine spindle. Carbides will stay sharp longer, of course.

I think the most important factor about the tool geometry is to select a "high-helix" endmill. Lots of guys rave about 3 flutes, but 2 flute may be adequate if you have limited feedrate capability on your machine. Lots of flutes is better for high feedrate finishing, maybe not so good for roughing (they may plug up...it depends on how good you can get the coolant into the tool.)

[MILLMANM]

Norman, at work we use a formula to run any endmill mosty carbide 2 flute but aluminun can be cut a a minimum of 400 surface feet a minute with carbide, hss cutters should run at 200 sfm most likely at your max spndle speed on small end mills less than 3/8
It goes somthing like this
surface footage * 12 / (3.14 * emill diam) = rpm
or 400 sf*12=4800
( 3.14 * .250) = .785
so 4800/.785 =6114 rpm

now you have the rpm to reach the sfm now the feed rate of the
end mill rpm*#flutes*chip load

rpm =6114 * # flutes 2 * chip load per tooth .002 is conseritive
so the feed rate would be 24.45

this is a good starting point and you can adj from there

Brad

[ngr1]

Thank you gentlemen!

After reviewing the specs of my machine I have discovered the Spindle Speed can range from 1100-10000 RPM.

[HuFlungDung]

And what is the maximum cutting feedrate for it? This is not the same as the rapid speed. Most all machines can rapid faster than they will reliably feed.

[ngr1]

Sorry, I should have included the full specs from the beginning.

MACHINE SPECIFICATIONS:
Maximum Travel Speed: 30 in/min.
Maximum Travel: X = 9.5", Y = 5.5", Z = 6.0"
Table dimensions 3 1/2 x 15 1/2 inches
Maximum Z distance to table : 8.0"
Z-Axis swivel 90 degrees
Mechanical Resolution: 0.0005 in.
Electrical Resolution: 0.00013 in.
Spindle Speeds: 1100-10000 RPM.
Rigid square tubular steel base and column construction.
X Axis - Hard Anodized cross slide table with 45 deg. dovetail.
Y Axis - Precisionly ground prismatic 90 deg. steel rail ways.
Z Axis - Steel box ways
Total Dimensions with motors 21" x 20" x 24".
Total Weight 85 lbs.

[bonz]

When it comes to machining aluminum, I have found that you will most likely be limited by your machine capability, not the cutting tool. If using solid carbide endmills, preferrably 2-3 flute high helix, with TiCN coating (less gauling and better lubricity), you can easily start between 600-1200 sfm. Feeds will depend heavily on cutter diameter and depth of cut (axial and radial).
Example 6061-T6 aluminum: periphery milling with a 1/2" diameter endmill 50% radial depth, 100% axial depth, you should have no problem running 4600 rpm (start) and feeding 30+ ipm (conservative).
It is essential that the workpiece be secure and not vibrate (carbide doesn't handle vibration well at all).
Caution - Start out more conservative if using some of these "incredibly priced" carbide endmills found in catalog flyers. I have found these to be very inconsistent.
Good Luck,
Bonz