I know that we have beat this to death..but

[ssutton]

I am cutting aluminum sheet on my 4X4 machine. I am using a Bosch 1617 router with variable speed (8000-25000 rpm). This model router has constant speed circuitry so that under load it will maintain the rpm setting.

The exact material that I am wanting to cut is 6061_t6 .032. My machine has vacuum hold down and it works great, so material hold down is not an issue. I want to cut thru this material in 1 pass.

I am using an onsrud O flute downcut bit with a 1/8 cutting diameter. So far I have not found an RPM/feedrate combination that prevented chatter/melting. The climb cut side is a much better cut but chatter is evident with you look at the finished profile. The conventional cut side is mostly melted and frayed.

I have cut up to 40 IPM and a RPM around 16000. And as slow as 10 IPM and 25,000 RPM. And just about anywhere is between. The results are not much different. I tried an amana up cut, but because the material is so thin the bit had a tendency to grab the material and pull it up on the edges, thats why I went to a downcut.

The next bit I am going to attempt is a solid carbide straight shank 2 flute 1/8 cutting diameter. I can not cut with anything bigger than 1/8" because I am drilling fastener holes with the same tool.

Does anyone know of any "secrets" to making this work? Is chatter just part of this? My machine is HEAVY and stiff, I don't think that the chatter is machine or material movement, just bit deflection. I REALLY DO NOT want to use any type of coolant because my vacuum hold down surface is MDF.


Thanks for your thoughts....

Scott

[ger21]

I have cut up to 40 IPM and a RPM around 16000. And as slow as 10 IPM and 25,000 RPM. And just about anywhere is between

The range you're trying to use is outside where it probably needs to be

Try 80 ipm and 12,000 rpm. I think the problem is that you're going too slow, with the rpm's too high.

[H.A.S.]

Use the tables of speeds and feeds for a beginning point only. Chip formation, (magnified), will usually tell you which way to go. I have had the exact same alloy cut differently, just because of humidity and/or temperature.

It's all a game of theory; what runs smooth as silk today, may be a bear tomorrow. Hope this helps.

[Pplug]

I am cutting aluminum sheet on my 4X4 machine. I am using a Bosch 1617 router with variable speed (8000-25000 rpm). This model router has constant speed circuitry so that under load it will maintain the rpm setting.

The exact material that I am wanting to cut is 6061_t6 .032. My machine has vacuum hold down and it works great, so material hold down is not an issue. I want to cut thru this material in 1 pass.

I am using an onsrud O flute downcut bit with a 1/8 cutting diameter. So far I have not found an RPM/feedrate combination that prevented chatter/melting. The climb cut side is a much better cut but chatter is evident with you look at the finished profile. The conventional cut side is mostly melted and frayed.

I have cut up to 40 IPM and a RPM around 16000. And as slow as 10 IPM and 25,000 RPM. And just about anywhere is between. The results are not much different. I tried an amana up cut, but because the material is so thin the bit had a tendency to grab the material and pull it up on the edges, thats why I went to a downcut.

The next bit I am going to attempt is a solid carbide straight shank 2 flute 1/8 cutting diameter. I can not cut with anything bigger than 1/8" because I am drilling fastener holes with the same tool.

Does anyone know of any "secrets" to making this work? Is chatter just part of this? My machine is HEAVY and stiff, I don't think that the chatter is machine or material movement, just bit deflection. I REALLY DO NOT want to use any type of coolant because my vacuum hold down surface is MDF.

Thanks for your thoughts....

Scott

I machine al by using a 1/8" 2 flute end mill and following this recipe:

Feed: 12 ipm- 20 ipm
Speed: 11280 rpm
Depth: .02"
Coolant: WD40
Direction of cut: climb milling

Watch out for melting, I have broken several bits in 6061 to find these settings. I also found that the first plunge cut is the hardest on the bit. Sorry to say this but you will probably have to do 2 cuts. I have never gotten perfectly clean results with a 1/8" bit however when I cut with a 1/4", I have a mirror like finish, of course with a different formula. I think that the 1/8" tend to flex more causing a rougher cut.

[louieatienza]

I have found that for profile cutting, I reduce my doc by half. I also use 1 flute spiral upcut bits by Onsrud and Amana. I find the Onsrud bits slightly better. Regardless, I almost never plunge in and almost always ramp in ehen pocketing or profiling aluminum.

I also find the speeds and feeds are somewhat proportional. My baseline is pocketing at 72 - 75 ipm, and 18000 rpm at 1/8" doc for a 1-flute 1/4" bit. So for an 1/8" bit I would pocket at about 36 ipm and 1/16" doc. For profiling I would do about 1/32" doc. You should use some kind of lubricant, and keep the kerf free of swarf. You should make sure that all your axes have tight movement, as any play will translate into vibration in your work. Also if your z is even the slightest out of tram, the bit will rub on one side on subsequent passes, which will heat up the bit. Also use a stub length if possible, or insert the bit as far in as possible. Lastly, make an auxiliary table that raises the workpiece up, since the less the z goes fown, the stiffer it is.

With my previous machine my feedrate is slightly slower, about 30 ipm:
[nomedia="http://www.youtube.com/watch?v=HhQ-NL5GGyA&feature=channel_video_title"]YouTube - ‪Milling Harley-Davidson logo out of 1/4" aluminum, part 3‬‏[/nomedia]

But I still got a good edge, despite having aluminum rails and skate bearings on a wood frame:
[nomedia="http://www.youtube.com/watch?v=u3Cyef85S6w&feature=channel_video_title"]YouTube - ‪Milling Harley-Davidson logo out of 1/4" aluminum, part 4‬‏[/nomedia]

Another example of profiling at 30 ipm, and about 1/32" pass.
[nomedia="http://www.youtube.com/watch?v=mAsp3_uN7SY&feature=channel_video_title"]YouTube - ‪Home Made CNC cutting aluminum clock gear 1/4" thickness Part 1‬‏[/nomedia]

If you find your still having trouble with the spiral o flute, Onsrud makes a soft O flute specifically for softer aluminum, though the smallest diameter is 3/16"...

BTW Amana recommends about 30 ipm at 1/8" doc!

[jsheerin]

Is chatter just part of this? My machine is HEAVY and stiff, I don't think that the chatter is machine or material movement, just bit deflection.
Scott

You don't say what your machine is, but I'll go out on a limb and say it's probably your machine causing the chatter. You need about 7x more stiffness for good performance cutting aluminum than for cutting wood, which is a lot. Your work holding solution is also part of that. What matters is movement of the material relative to the cutter. You can get by with all the tips you've just been given (it's how I do it as well), but lack of stiffness is likely the root cause.

[jharvey407]

I have been using a simple test to determine appropriate feeds and speeds that you may want to try.

Pick your material, RPM and endmill.

Program a zig-zag with legs about 2 or 3 inches long. Start with a reasonable feed rate, perhaps 10 ipm. Program your zig-zag so that the feed rate increases by a set amount for each leg, maybe 10 ipm. Program the zig-zag to give you a reasonable range of feed rates.

If you program 10 zigs and zags, you can get feed rates from 10 ipm to 100 ipm. Run the program and watch the cuts. You will see a noticeable improvement in the finish as the endmill approaches it's optimal feed rate. Once the finish quality starts to degrade you know you are pushing the tool to fast.

This should give you a good starting point.

[louieatienza]

Another thing is spindle power. I also use a Bosch 1617EVS, but I have the speed control removed, and control the speed via a SuperPID. While the Bosch does have constant speed circuit, it is not nearly as fast, and doesn't provivde the motor with as much juice at lower rpms, than the SuperPID. Another benefit of the SuperPID is I actually tweak the speed slightly to find a "butter zone" where I can feel the router vibrating less and the see teh chips streaming away from the bit; and the chips will be pretty hot.

There are many videos on YouTube of huge VMCs milling aluminum with 1/8" bits and leavivng excellent finishes, but these machines have upwars of 5jp to even 20hp spindles. And all those machines are heavy cast iron, run with servos.

You do not mention what kind of drive system you have. I would also check for any backlash. Another thing you can try is make a special platen for you vacuum table to place your workpiece on, that has a groovev or channel at the profile line so that the chips with the downspiral bit have a place to go to, instead of becoming trapped. As for lubricant, you really don't need a lot at all, just a fine misting with WD-40 or even liquid wrench would help.

[ssutton]

You don't say what your machine is, but I'll go out on a limb and say it's probably your machine causing the chatter.

Could be, my machine is a one-off design. I even designed the linear bearings and rails. That said, I design machines for a living as an automation engineer and the machine is pretty stiff and rigid. The drive is R&P and at certain speeds I am having jerkiness or lack of smoothness. Gecko techs seem to think that it may be mid-band instability and that it could be tuned out. I can visually see the jerkiness in the 60 to 90 ipm range, but it may be happening at all speeds and I just can't see it. That could be causing a lot of my issue. I have eliminated most of the issue by running up the acceleration and deceleration values so that the machine will pass thru this speed area much faster. Assuming that my machine is not the issue, I really wanted fresh input on the subject from you guys that have been there and done that.

Thanks for everyone's thoughts so far

Scott

[jsheerin]

If you design machines for a living, maybe you already know this, but you want it in the 20,000 lbf/in range or higher between the work and the spindle nose for aluminum, and ideally a primary resonance in the 30Hz or higher range. This would include the stiffness of all the bearings and rack and pinion mechanism in case you want to do some fea on it. I know my router is in the 1k-2k lbf/in range from measuring it, so it doesn't surprise me that it doesn't have the best surface finish on aluminum. If you want to measure, you can use a fishing pull scale and dti for a quick number. The VMC's louieatienza refers to can be in the 50k-700k lbf/in range.

[RomanLini]

...
The exact material that I am wanting to cut is 6061_t6 .032. My machine has vacuum hold down and it works great, so material hold down is not an issue. I want to cut thru this material in 1 pass.
...

... I tried an amana up cut, but because the material is so thin the bit had a tendency to grab the material and pull it up on the edges, thats why I went to a downcut.
...

I know you said your vacuum holddown is good, but wanted to throw my opinion in too.

If you are cutting right through in one pass there are quite strong forces on
the material, and that is a thin and springy type of aluminium.

So even if your vacuum holds down the bulk of the material the edge where all the cutting force is can still deflect (bend up) and vibrate etc.

I'm not going to pretend to be an expert on cutting aluminium but on my machine I never cut all the way through on one pass. I cut most of the way through and leave a small "skin" holding the metal together this provides a surprising amoung of support all the way around the parts to stop vibration and climbing (and aid a vacuum seal in your case).

Then a second pass cuts through the thin support skin, as this is thin (small DOC) it needs very little force so it won't deflect the sheet much at all.

Although it sounds like more time taking 2 cuts you might benefit from being able to cut the first one more agressively (as it's better supported) and the second cut being very thin can be done faster anyway.