machining 6061 aluminum

[conlimon]

hey all -

i'm a newbie with my Taig 2019 er16 setup from Deepgroove1, and i'm having a bit of trouble getting aluminum to machine nicely. I've been building parts out of acrylic with no trouble, and the machine setup seems good. when i cut aluminum, i feel like some of the chips are getting embedded back into the work, creating a rough looking cut. i guess i'm asking about a starting point for spindle speed, feed speeds, and depth of cuts to get a high quality machined surface. the result i'm having is that when i cut a groove with a square endmill, the sides of the cut are sort of rough. is this normal?

any help would be greatly appreciated. just as a point of reference, i'm using my Taig to build parts for the aircraft that i'm building. my website chronicles the shennanegins here... www.perfectlygoodairplane.net
for any interested. some of my early attempts at using the mill are pictured here:
http://www.perfectlygoodairplane.net...op%20Mill.html


thanks!
cj

[mark c]

Hi CJ
Looking at your pics, It looks like you are cutting dry. With al you need a coolant/oil otherwise it will gall. Use WD 40 if you have nothing else, but you can get a coolant mist system from www.littlemachineshop.com for pretty cheap.
It also looks like you are conventional cutting. To cut the outside of a feature you should go clockwise and on the inside go CCW. This will give a better finish. It's also best to leave .01" on the side and take a finish pass.
That said, a surface speed of 350/450 for a high speed steel end mill is a good starting point, for a 3/8 end mill that is from 3565 to 4583. 1/2 is 2673 to 3437. Depending on the rigidity of the mill (don't know much about Taig) the feedrate will be RPM *.002(+or_)* the number of flutes on the endmill. This can vary widely, but start at .002 and work up or down. For just cutting the outside of a part when the endmill is fully enveloped in the material, I would go no more than 1/3 than the diameter of the tool deep per pass. Depending on the rigidity of the Taig it could be more or less, probably more toward the lesser side.
Hope this helps. It would be a good idea to blow out the cutting area from time to time, but if all you have is a vacuum, then use that.
Let me know if you need more hints and good luck

[warossignol]

If you fly cut try putting a small radius on the bit tip.

[warossignol]

If you fly cut try putting a small radius on the bit tip.

[scubasteve_911]

Hey CJ,

First of all, I'm not a master machinist, but I am a pretty logical person and I have been using the Taig for a few months now.

When we first started out, we used four-flute endmills for cutting into the 6061 aluminum. Big mistake! Stick to 2-flute endmills if you can, the're very good for aluminum. Otherwise, the four flutes can get clugged and chips compact in there, then that's what causes a terrible finish and potentially an endmill break depending on diameter.

I use Mastercam for generating toolpaths and I stick to their recommended spindle speed and feedrates. These can be calculated easily, but I'm too lazy. The rest of the poor finish problems originate from chatter.

Suggested Modifications for you:

1) Use isolation vibration standoffs for the induction motor, available from McMaster-Carr, I forget the part #

2) Bolt that baby down to something big and heavy ( i used a 100lb concrete slab )

3) Use some of that white dryer tubing to make cheap bellows to better protect the leadscrews from chips, or go all out and spend 500$ on proper bellows.. I'm happy with my fairly ugly 5$ solution

Steve

[conlimon]

that is all excellent info - many thanks to those who posted. i'm cutting some stuff this weekend, so i'll give the suggestions a try, and report back!

cj

[mxtras]

At least use an air blast to keep the flutes clear. Direct the air to blast the chip out of the flutes as soon as possible. Of course, this is easier said than done, so multiple nozzles are always helpful. You can make a manifold and use small diameter brake lines or copper tubing to direct the flow and create some flexibility.

One trick to determine speed/feed is to measure the chips coming off the cutter. If they are not coming off the cutter, that's a big problem. Anyway - the thickness should be somewhere around .006" to .007" max for tools smaller than about 3/16" and somewhere around .009" - .010" for larger cutters. These are my guidelines. Always try to use the largest tool the part will allow. The larger diameter will not lolipop as easily since they typically have better flute shape and volume.

Scott

[scubasteve_911]

I think he is already doing something similar by holding a shop vac right onto the workpiece while milling. I like your idea about the tubing, it would be fun to make a shopvac attachment that you can run to a semi-rigid pipe then have directly over the endmill.

CJ,

I forgot to mention you can buy high-helix endmills especially made for aluminum, but they're too much money for my blood.. If you check out an ebay store called Discount Machine Shop, he sells 8% cobalt endmills (either 2 or 4 flute) with a 3/8" shank and various cutting tool diameters for dirt cheap. I buy all my stuff from him, $3.50$ is hard to beat for an endmill

Steve

[mxtras]

I really don't think a vacuum is going to provide enough pressure to blast the chip from the flute of a rotating cutter. My suggestion was to use the force of the air blast to clear the flute - not to simply clear the path of chips. The chips tend to want to stick to the flute right at the cutting edge. As the cutter rotates, the next cut on that flute welds the sheared aluminum to the previous chip and the cycle continues until you have a spinning aluminum lolipop.

Using an air blast should be a second choice to flood or mist coolant for aluminum but it is effective for small diameter tools. Air volume is not critical - a directed pressure stream is the key.

Scott

[scubasteve_911]

Ahhhh, I gotcha, I didn't think air would provide adequate pressure because if a chip gets compressed on there, it takes a hell of a lot of force to get it off.

Steve

[mxtras]

That it does. If it is stuck on there that well, your feed/speed is way off.

With good chipload, the chips will pretty much fly off like they do milling any other material (well, almost). Over a short period of time, there will be build up on the face of the flute when cutting dry.

Like I said - measure the chip thickness. Just as when drilling, focus on making a good chip and treat the cut as a byproduct rather than the other way around.

Scott

[ZipSnipe]

Mxtras makes a good point. However you didn,t say if you were face milling or pocket milling. With face milling a carbide face cutter(if they have one for a Taig) is the way to go(and you could use it dry). For pocket milling flood coolant is the preferred way to go or at least use the blast of air. We mill lots of aluminum where I work and those are the two methods we use.