Re: CNC Tooling
 

Don,

Look at the Onsrud catalog - the 63-600 product line is probably what you want to pick up. McMaster sells them if you search for "Router Bits for Aluminum" - "Grooving and Slotting". They're 1 flute solid carbide. The biggest issues with routers are going to be chip evacuation and and getting lubrication on the tool.

The 1-flute tools are nice because they give plenty of space to evacuate chips, and you don't have to run them at a high feed rate to maintain a proper chip load on the cutter to prevent it from rubbing. Depending on the construction (ball screws? rack and pinion?), your machine will probably be happier at lower feed rates and acceleration rates.

You'll definitely need something to get evacuate chips and provide a little lubrication on the tool. Otherwise you'll be re-cutting chips and getting a built up edge on the cutting tool - leading it to load up with aluminum and come to an untimely end. We're picking up a micro-drop coolant system (Trico Md-1200), which is like a mister, but instead of a constant stream of mist, it shoots small droplets of lubricant along with an air blast. They're more expensive than mist systems, but seem to clear chips better and don't make as big of a mess. Regular misting systems tend to linger in the air, and breathing that stuff isn't the greatest. At the very least look into a Fogbuster system to minimize that, or good ventilation.

Re: CNC Tooling
 

Second the Onsrud single flute cutters. They have been life-changers for our CNC Router. We run our spindle at 18,00 RPM with these same 63-XXX series Onsrud cutters, and they are incredible. Chip clearing performance was key in getting nice finishes on our cuts - and the feed rates we can run with these cutters are pretty aggressive too.

Our CNC Router came with a Unist Mister as an option, and we consider it a must when cutting aluminum. Mr. Stehlik here at 610 has been a big fan of the mist coolant approach and Unist misters in general, and has outfitted our metal chop saw, mill and lathe all with similar Unist misters. I don't think we've used a bottle of coolant all year long, clean-up has been easier, less machine corrosion, and the cut qualities have probably been better overall.

Here's a link to our Canadian supplier for the Onsrud cutters:
http://www.cncroutershop.com/ca/inde...us-metals.html

A not very useful picture and description of our router's mister setup from the manufacturer:
http://www.axyz.com/us/secondary-options/
...but if you read between the lines, it setup not as a continuous mister, but as in the post above it periodically dispenses droplets of coolant through a pulse generator.

A link to Unist's line-up of misters:
http://unist.com/solutions/machining-cutting.html

Re: CNC Tooling
 

We got a box of roughly 100 1/8" bits for our 4' by 4' cnc router to cut sheet aluminum. Our sponsor gave us the box several years ago, and we've only broken a few and we've cut a TON of sheet metal. The bits are similar to 3317A21 from mcmaster, but they are a little different, and the writing on the box is in Chinese. The trick is to get the feed rate correct, and have an air line always pointing at the bit.

Re: CNC Tooling
 

Thanks for all that info, especially the mister and lack of need for fluid collection - it seems that's the way to go.

6 IPM? gee, that's really quite slow. I expect to be cutting several tens of inches per minute. Maybe my mileage will vary...

The minimum speed I can get is 8000 RPM.
OK on Omsrud, I have heard this from others as well.

It is a Rack & Pinion machine, with an integrated dust (chip) collection system and safety shield (using a 2-1/2" vacuum hose), which I hope will deal with both the mist vapors and chips. And dust, when I cut anything not metal.

Any comments on which cooling fluid you use? There are so many choices...

Re: CNC Tooling
 

Have you checked out the math for calculating speeds and feeds? 2000RPM and 6IPM is way too slow, that's only 0.001 in/tooth. Way too low for a 1/4" end mill.

Spindle Speed is roughly the surface speed (in feet/min) * 4 divided by cutter diameter. Carbide in aluminum numbers can exceed 1000 SFPM, so you can run up to at least 16,000 RPM with a 1/4" cutter. You can run slower with no ill effects here, might want to check out where the peak torque or efficiency is on your router.

Feed rate is the chip load * #teeth * spindle speed. Here's the link to the Onsrud specs. They don't provide a SFPM rating which is odd, they just list 16,000 RPM.

http://www.onsrud.com/files/pdf/2012...20Aluminum.pdf

They list 0.003-0.006 in/tooth for 1/4", you don't want to have this drop too low or the cutter will just be rubbing as opposed to taking a clean chip. Plugging those in gives you 16,000 RPM and between 48 inches/min and 96 inches/min as your feed. If your machine is unhappy accelerating that fast - just drop the spindle down to 8,000 RPM and feed between 24 in/min and 48 in/min.

I like the calculators at this site - they have one for HP/Torque requirements also that will let you get a feel for how heavy your cuts are.

http://www.custompartnet.com/calcula...speed-and-feed

G-Wizard is another nice (pay) piece of software that gives some good suggestions and does fancier stuff like calculating tool deflection on smaller cutters.

http://www.cnccookbook.com/CCGWizard.html

We use KoolMist 77 as flood for our mill (McM 11365K61), but it obviously works as mist as well. It's probably not the ideal coolant for aluminum, but it's one of the safer ones to work with. The MSDS sheet is pretty tame, it doesn't go rancid in the tank, water soluble, no skin reactions, biodegradable, etc.

I would just take the dust-shoe off when you're cutting aluminum, it'll get in the way of the coolant system and you won't be able to see the cut. Bump up the pressure in the mister so that it clears chips from the slot, or mount up an air blast. A lot of milling in steel and hard alloys is now done without coolant, just a heavy air blast to clear chips and prevent recutting. Aluminum needs the lubrication though.

Re: CNC Tooling
 

Yes, 6 IMP. We do throw a good chip though, nice little curls. It is quite slow, mostly because we have a mill mentor who is, shall we say, conservative, with his machine's speed. He is right to go slow, though, the chips look good and we have had problems with breaking tools in the past (and crashing into clamps, but that's another story).

I'm sure with those router speeds, you'll be able to go faster. We're running a very different type of mill (a HAAS toolroom mill), so take my cutting speed experience with a grain of salt.

Perhaps we do cut too slow, but since the chip looks good and our part tends to vibrate excessively if we push it much faster, I'm inclined to stick with what we have now.

Re: CNC Tooling
 

A HAAS TM should be able to go faster.......... we were cutting up to 30IPM on ours in Alum with no problem.

What kind of spindle speeds are you spinning at?

Re: CNC Tooling
 

Are you using carbide or HSS? With HSS I could see 6 IPM being reasonable, but you should be running at about 0.003 IPT or more with a good carbide end mill, which would be a baseline of double what you're currently running. With a cutter that small and a top speed of 3600 RPM I would never run slower than max speed. We were forced to run our machine no faster than 2500 RPM recently and were slotting 1/4" plate at 23 IPM with a 3 flute end mill. You have a less rigid machine, but 1/4" Al plate isn't very taxing and I would expect similar performance.

As Scott mentioned, with a chip load of 0.0015 IPT you're coming closer to smearing material off as opposed to shearing, which will dull your tool and cause premature breakage. This will be a bigger problem if you're conventional instead of climb milling as chip formation begins with zero thickness and increased rubbing.

If you find that you're breaking tools it's almost certainly a chip evacuation problem. We can slot 1/4" plate with a 3 flute aluminum specific end mill indefinitely as long as the chips are cleared out of the path of the tool. As soon as you start re-cutting chips you run the risk of dulling/snapping the tool or welding the chips to the flutes.

Re: CNC Tooling
 

Like I said, somewhere in the 2000-3000 rpm range.

Re: CNC Tooling
 

Just for perspective, whenever I CNC using a 1/4 HSS EM I run the spindle at 2500 rpm and cut at 10 IPM. For me HSS doesn't chatter till you get up around 20IPM, if you're chattering at 6 IPM you might want to look into your fixtureing and make sure you've got a nice sharp endmill.

Re: CNC Tooling
 

Most of our cutters are HSS, but I believe we have a few carbide tools. We tend to really only push up to that 3600 limit when using 3/16" end mills or smaller and small diameter number drills.

This whole discussion of our cutting rate leaves me rather wondering if our mill has been incorrectly displaying units for cutting or something... I was always told that the units for the feed rate readout were in inches per minute. Like I said, we usually cut with that in the 2-6 range. I think we've pushed it up to 10 or 12 in the past, but that introduced some very serious vibration, and I believe even some tool deflection. Cory, maybe you're right, maybe this is all caused by a less rigid table, and our low cutting feed rate is just a product of vibrations occurring when we get near "normal" cutting speeds.

We have experienced some dulling and tool wear. Perhaps this is due to the lower cutting speeds we use wearing instead of cutting. When we increase spindle speed and cutting speed, though, we tend to start melting chips onto the tool. I always attributed this to poor cooling (even with the mist coolant) rather than chip evacuation or low cutting speed. We always (well, except for a few special cases) climb mill.

Granted, when I'm talking about tools breaking, I'm talking about a couple of 3/16" or smaller endmills breaking when they took too deep a cut at too high a feedrate.

Re: CNC Tooling
 

Feed on a mill is displayed in inches per minute, but it doesn't mean much without knowing the chip load which is in inches per tooth. Chip load is independent of number of flutes, which makes it easier to talk about as a comparison.

Re: CNC Tooling
 

Most work I do with a 3 flute carbide 1/4" endmill with flood coolant is at 6000 RPM and around 40-50 IPM depending on stepover and depth of cut, and I bet I could feed a good deal faster than that. I slow it down to about 20 IPM for a 2-flute ball endmill.

On our router, I'm running about 18,000 RPM on a 1/4" 3-flute carbide, and cut around 12 IPM (and much lighter cuts too) but that's due to a lack of coolant of any sort, poor chip evacuation, and chip recutting which is causing a heating issue.

A machinist I work with is running a 1/4" 3-flute tool at 12,000 RPM and 350 IPM (with flood coolant of course) with a 1/4" DOC and high-speed machining toolpaths with probably 25% stepover.

Re: CNC Tooling
 

I uploaded a machining calculator called ME consultant to the CD media section. It's a great simple freeware tool to find out basic speeds and feeds.

Enjoy

Re: CNC Tooling
 

Thanks for that coolant info Scott. "Rancid in the tank" is a real eye-opener for me. Oh, and the dust shield is clear plastic, so seeing the cut isn't a problem.

DampRobot, 6 IPM is 1" in 10 seconds, or 0.1" per second. Just seems slow to me, but....

1. You're getting good results. Something must be right, eh?
2. What kind of depth of cut we talkin here? 0.1" or 1/2"? That matters...

Anyway, I keep looking at #1 above and concluding it's OK.