[Cowbell]

Yet another newbie question. Flipping through the posts here, and reading the textbooks, I always see RPM numbers for milling aluminum that are well above what my Grizzly mini-mill can do. It tops out at 2500 RPM. But I always see RPM's in the 4000+ range being quoted.

Main point: As a beginner, I'm looking to figure out my technique to get nice clean cuts with no welding and minimal surface ugliness. I don't mind feeding slow.

Assuming liberal amounts of coolant (I'm rigging up a flood cooling system, flushing Kool Mist mixed 1:4 with water) and relatively slow feed rates (<= 12"/minute), what's the no-brainer approach for me? Always crank the mill up to the max (2500 rpm) and feed at whatever I feel comfortable with? Or keep the RPM's down in the ~1000 range, because at that feed rate range it just doesn't matter?

[chineguy]

When cutting aluminum use High speed steel cutters. Preferably 2 flute cutters designed for aluminum. The general use type cutters meant for steel will clog and pack up solid very quickly. 4 flute HSS cutters will also clog even faster. They can be used with very shallow depths of cut and low feeds in a pinch, but don't turn your back on it. Don't even think about carbide on such a slow spindle even if the cutter is designed for aluminum. Crank up the speed but you might get a lot of vibration on a light duty mill. The softer grades are easily cut at 400 Surface Feet Per Minute and up. I have run 1/2 inch end mills at 4000 rpm and 60 inches per minute .100 depth of cut on a Lagun mill with Prototrak MX3 control. This is a far heavier machine than yours. It is still a light machine by industrial standards though. Using flood coolant can be messy when cranked up like that. We used an air blast or mister most of the time.

[mrainey]

The only negative to the slower RPM's are fewer inches per minute of feedrate. If that doesn't matter to you, run slower. You'll probably make less of a mess and your spindle will last longer.

[NC Cams]

Multi flute cutters always have one flute a teeny tiny bit higher than the others. THus, it will always cut more/heavier than the others. Even so, you have more teeth in contact with the part which evens out the stress loading of the tool and it deflects less than the interrupted cut of a 1 or 2 flute cutter.

The key to good surface finish is:

1. More flutes in contact with part keeps the tool loaded more evenly than single or double flute cutters - less chatter potential for better finish.

2. Low feed (in/min) rates lets the cutter make more passes over the surface thus a smoother/finer finish.

3. high surface footage (SFM) does same as 2 above.

4. Light cut depths offer less tool load/deflection/chatter potentia and also apply lower shear stresses to the parent metal.

To wit, we finish mild steel disk masters with 1.375" HSS cutter, 6 flutes at 130rpm and 1.5"/min with 0.002" stock removal on final finish cut. Coolant is Valentite VNT700 + water.

Finish and accuracy is very close to that of ground part after you buff it with scotchbrite.

[little bubba]

I don't mind feeding slow.

Give it some time, you will mind feeding slow. From your post, I get the feeling your hung up a bit on RPMs, you need to get your brain in the mode of thinking Surface Feet per Minute. The RPMs you need are then determined by your SFM. Since you didn't give a cutter diameter or a material, though I'm assuming aluminum its actually impossible to recomend an RPM or feed rate.

Also don't get hung up on inches per minute, think of chipload per tooth, and use that to calculate your feed rate.

As for the previous advice given I'm going to disagree with some of it. 2 fluters are great for roughing aluminum, but when your finishing, you don't need the clearance for chip evacuation, and the extra flutes will allow you to feed faster. On the same note, even for roughing once you get to 3/4 and over, I find a two fluter to be overkill, a four fluter generally will provide plenty of chip clearance.

As for not using carbide at low speed, I do it when I have to, and when run at HSS speeds will last damn near forever, provided you don't let it get into a chatter situation. Also carbide for your small endmills can't be beat due to the rigidity of the cutter, and 1/4" and under carbides are dirt cheap.

As for spindle speeds, 1/4" HSS endmill in aluminum at 600sfm is a bit over 9000 rmps. a 1/16" carbide in 1018 at 300sfm is 18000 rpms. Doesn't take much to need a higher spindle speed.

[miljnor]

we finish mild steel disk masters with 1.375" HSS cutter, 6 flutes at 130rpm and 1.5"/min with 0.002" stock removal on final finish cut. Coolant is Valentite VNT700 + water.

Finish and accuracy is very close to that of ground part after you buff it with scotchbrite.

sounds too good to be true!

How long does your cutter last??

With this small of a chip load I would guess that recutting small chips would fracture the edge of the tool make lines appear in the material????

But I have never tried it.

[DareBee]

I have to agree with Bubba. Especially on the carbide. Pricing on carbide cutters 3/8 and smaller is so close to HSS price that it is well worth it, rigidity and deflection are the main reasons to use carbide for small diameters.
I personally have found that regular carbides dont last much better than HSS but get a Ticn or Tialn cutted carbide and the cutter life goes up 100 fold when run properly in a CNC. Tialn will machine hardened steel up to about 60Rc fairly effectively as well.
As far as aluminum goes I will only use 2 flute for small (under 1/4) slotting and even then it has to be deep for me to switch, you get twice the feed out of 4 flute.
Any speed charts I use for cutting show Aluminum with a carbide cutter listed at "Max RPM" (obviously not a 6" facemill) in my case 10,000.
Example- 3/8 Tialn "Ultra" 4 flute 10,000 RPM 86 IPM feed
at 2000 RPM keeping the chipload at .0022 feedrate = 17.2
The cutter does the same work with the same stress 5X SLOWER
BTW in this example I probably should even have a 15K spindle but I am even running slow my SFM is 980 here and should be about 1100