need help cutting ALUMINUM. thank you.

[max90272]

HI guys,

I'm a newbie at CNC machining. I have built a 3-axis desktop CNC machine and I have now been using it for about 2 weeks with MACH3 which I love (still the demo version but planning to buy). Here's my thing.... I'm a little puzzled as to how to cut aluminum!!!! I have my dremel tool as a temporary spindle just so I can understand how MACH3 works. Of course that tool can turn up to 35 000 rpm which is really high and I have bought 2 mill end cutters of brand ATRAX made in the usa, which I believe of good quality. They are both 1/8' dia. and one is 2 flute the other is 4. I figured with that set up (good speed, good quality end mill ...) I would be cutting through 6061 aluminum like butter but I find myself having to constantly reduce the feed rate to avoid MAJOR tool crashes. I am using lubricant to help to process and I have tried slow and high speed on my dremel but still it takes FOREVER to cut a 1" circle in 1/4" thick aluminum.

Is this slow cutting the results of using a small diameter tool? If I used a 3/8 end mill, wouldn't it be even slower because of all the extra material to cut?

I am reaching out to you guys because I have exhausted my resources. Is this normal to cut that type of material so slowly? That makes me wonder how high-speed machining works... I am puzzled ... please give any advice.

Warm regards

MAx

[Jason3]

Hi Max,

You'll need to match your RPM to feed speed to get the right chip load - for that size cutter I'd suggest keeping feed per flute to between 0.002" - 0.0015". So, say you run a 2 flute cutter at 30,000 rpm that's 2 flutes x 30,000 = 90 - 120 IPM feedrate. If your machine won't run that fast, reduce RPM as needed to maintain the right chip load.

Also, with a dremel, you will need to take light cuts - I'd suggest .01" DOC per pass, since the dremels usually have the bearings mounted in plastic - not the most rigid setup.

Are your Atrax cutters the carbide ones? I use them - they go pretty well for me. Here's a link to a vid of my machine using them (I have posted this before on the Zone, but I'll put it here too, since it illustrates the technique I'm suggesting you use. This is at about 100 IPM, 30,000 rpm and a 1/4" 2 flute Atrax carbide end mill, .01" DOC):

YouTube - CNC milling 6061 aluminium

YouTube - CNC milling 6061 aluminium

Best regards,

Jason

[HuFlungDung]

High speed machining works, but requires more horsepower. In aluminum, you need to keep the feedrate up, otherwise, you drastically increase the heat being generated in the cut zone, which makes the material gummy and the chip wants to weld to the tool, which then cannot cut and it breaks off.

So with a Dremel (perish the thought ), you'd need a really shallow depth of cut and keep moving right along at a high feedrate, kind of like a mosquito buzzing around your head

[max90272]

WOW Jason, that is some fast machining there!!! How are you able to cut like that without lubricant? I thought it was not recomended. What is the final verdict on cutting dry versus lubricant??

If I'm not mistaken, you are suggesting to keep a high feed rate for 6061 aluminum, but with VERY THIN layers removed (it looks like the proper term for layers is DOC, is that correct?). In other words, more passes, thinner depth each pass??

The way I had MACH3 programmed for my job was with 0.08" depth per passes. . Is this why I had to slow way down my feedrate to avoid crashes??

I am also confused with the chip load you mentionned. What is the chip load exactly and how do we calculate it?

Thanks again everyone.

[Jason3]

Originally Posted by max90272 WOW Jason, that is some fast machining there!!! How are you able to cut like that without lubricant? I thought it was not recomended. What is the final verdict on cutting dry versus lubricant?? If I'm not mistaken, you are suggesting to keep a high feed rate for 6061 aluminum, but with VERY THIN layers removed (it looks like the proper term for layers is DOC, is that correct?). In other words, more passes, thinner depth each pass?? The way I had MACH3 programmed for my job was with 0.08" depth per passes. . Is this why I had to slow way down my feedrate to avoid crashes?? I am also confused with the chip load you mentionned. What is the chip load exactly and how do we calculate it? Thanks again everyone.

Thanks! That machine is quite a light one actually (it was my first ), but it will happily feed at twice that speed (5,000 mm/min - 200 IPM). I don't like to run that fast the first time I run a particular part program though - if I stuff up the G code I can't stop it quick enough!

Dry vs. cutting fluid - well, there are valid reasons for going either way. Generally, using coolant will help prevent the chips heating up and welding themselves to the cutter. It also reduces the force required to push the cutter through the material, and helps clear the chips out of the path of the cutter. Personally, I don't like cleaning it up, that's one reason I tend not to use it.

High speed dry cutting relies on several variables to work well. First and most important is the Chip Load you were asking about. This refers to the amount of material removed by each flute on the cutter each rotation. Contrary to what one might at first expect, too little chip load often causes more heating than too much. What happens is that the cutter heats the material each side of the cut. Half the heat is disposed of with the chip. Then the next flute on the cutter removes the hot part of the material and so removes the residual heat from the previous cut. In this way the majority of the heat from the cut is disposed of in the chips. When the chip load is too small the hot area extends past the material removed with each flute, and the heat builds up until the material starts to melt and weld itself to the flutes. Coolant can help prevent this.

You're right - I'm suggesting high RPM, brisk feedrate and small DOC (depth of cut). Get that chip load up! As Hu said, keep the feed rate up, a common mistake when having difficulty cutting is to crank up the revs and reduce the feed.

In your case, you want to compensate for lack of horsepower with the light DOC. In doing this you are also compensating for the lack of rigidity in your spindle, reducing the force required to push the cutter through the material and so reducing the deflection, which helps keep the chip load constant. So yes, .08" DOC was not wrong in itself, but a dremel is not the spindle for that - not rigid enough and not enough power.

So, you don't so much calculate chip load, but rather feed rate and RPM. The cutter manufacturer should state the recommended feed per flute for your cutter - I don't know whether the spec for Atrax is available online or not. If not, try starting between .001" and .002" per flute. Your dremel will probably make the most power near it's max. rpm, so start there to calculate feed rate. Say 25,000 rpm (remember it will slow down under load), x 2 flutes? x .001" - .002" chip load per flute = 50 to 100 IPM (inches per minute). If your machine won't run that fast reliably, then start the calculation with your max feed rate and work out the RPM you need to get the chip load within that .001 - .002" range. I'd start with a .005" DOC and work up from there if that goes well.

Sometimes success depends on trial and error. If you get chatter, try dropping the RPM slightly. Don't have the cutter any further out of the chuck than you have to for a particular job, or to keep from gripping the flutes. You could consider getting a couple of stub end mills for the 1/4" alu sheet - the closer you can get the point where you are cutting to the spindle bearings the better you finish will be. If the chips aren't being thrown clear by the cutter, make sure you get them out - recutting them uses power you can't spare. I use a fan to keep the part clear, the speed of the cutter does most of the work.

Let us know how it goes!

Best regards,

Jason

[neilw20]

This is my opinion. Feel free to correct me.
When cutting there is a load against the cutter, (and it also may not be in the direction of the cut). This load deflects and bends the machine and can put a bending load on the cutter as well. When the totals of this deflection approaches the feed per tooth/flute the cutting action becomes unstable and this becomes apparent as chatter. Reducing the DOC (Depth Of Cut) reduces the load on the cutter and hence the bending. This reduction in load reduces deflection of the machine (which maybe as simple as bending of the spindle shaft).
Deflection of the machine becomes more apparent pushing BIG cutters which may not bend as much. It all comes down to stiffness of the whole system.
The high speed works well because it keeps the deflections caused by chipload below the actual chipload.
It is important that the cutter does not eat it own chips, but when the chips are tiny they don't cause as much problem, and can be blown away.
There is also resonant cutting utilizing these deflection mechanisms to advantage, but that's above my 3500 RPM so I can only wish.

[Jason3]

Neil - I'd agree with you - that explains why commercial VMC's are so massive. Would you have some comment on the advantages/disadvantages of using coolant?

Max - what type of machine have you built - is it a gantry type router or a vertical mill type? Neither?

Regards,

Jason

[neilw20]

I use coolant when it won't work dry. Often flooding keeps the small particles from being recycled by the cutter.
Also stops chips getting clogging the cutter.
A dry option for aluminum is candle wax. Can stop files clogging too.
Ideally, most of the energy ends up in the chips as heat, and the works stays cool. With some material like K1045 big blue chips blown away with air works.
Add coolant and the chips heat treat themselves, and straight away HP goes up 3-5 times overloading my 15KW motor ! That stuff needs air, but boy is it noisy !
Hand brushed kerosene on aluminum is good. Too much is a fire hazard.
Different materials need different coolants. Consult your tooling supplier specialist. Magnesium is an interesting fire hazard.

Neil

[max90272]

Thanks guys,

Jason... tell me you didn't build that machine yourself... I won't believe it if you did. It's amazing! I definately need to stay in touch..... Which state are you in?

My machine is a vertical mill and i have attached a picture. The stack of wood on the x axis is just temporary while I am testing the software. I have yet to build a mill table. The sharpie on the Z axis is there just for use of testing as a guide, and i got rid of the dremel that was sandwiched there between the 2 wood plates. I have a real cast iron spindle but no motor and still figuring out how to rig it.

[max90272]

Hey again,
So basically a 4-flute cutter should get twice the feedrate of the 2-flute one at same rpm? Is this right?

[Jason3]

Hey Max,

That looks like you have some pretty decent travels there! Are you going to beef up the base and column at all? Your cast iron spindle might make it flex a bit.

Yep, I built it - the machine in the video is not the one in my pic by my username, though I made 'em both. There's a third one on my desk which is also nearly finished too. Can't wait to try it out, I think it will look nice on the coffee table in the living room

I'm in New Zealand, a small island nation in the pacific (not far from Australia) which is usually very nice but lately is getting an awful lot of rain...

And yes, 4 flutes = twice the feedrate of a 2 flute cutter, as long as there's enough clearance for the chips to clear.

Neil - you wouldn't happen to have a video clip of that blue chip K1045 machining you mentioned? I'd really like to see that, I like watching that kind of serious metal removal. It makes me want to build a real, heavy machine...

Best regards,

Jason

[neilw20]

That job,which went on for years on an OKK (6MG I think) is now finished.
It machined dies for a not so green, carbon intensive part of the electricity system wearing spares, and like most contracts, eventually moves or ends.
Same machine was used to drill 40" long 3/4" holes at about 1.25IPM./ 1200 RPM fixed gun drill, that X-axis on the OKK moved the job to the drill.
Drill was rigged on a modified portable 2 ton horizontal borer. 7.5HP 1200 RPM
7HP compound pump running 600PSI. Splash guards were important !
All history now.