13 replies to this topic

[Marshal]

I'm trying to get into using our CNC router to compliment our mill a bit, so I tried actually machining some 6061 aluminum with it today and the finish didn't come out nearly as nice as I'd like.  There seemed to be a lot of tooling marks on the floor of a pocket, and a heck of a lot of chatter on the walls.  I tried multiple 1/8" cutters, a single flute straight, a two flute helix, and a four flute helix endmill and they all came out with similar results.  I tried doing a parallel spiral-clean corners as well as dynamic milling.  They all seemed to have quite a bit of chatter, which in part I assume is from the router not being nearly as rigid as something like a VMC.  

I was running the machine at 20k RPM, and had it set for 200ipm but I know it doesn't get anywhere near that since it takes a little distance for the machine to ramp up to that feed.  I'm sure part of it comes down to getting feeds and cut depths right, but I tried multiple ways, from 0.150" deep to 0.020" deep, with a 10% stepover and using a 2D contour as like a 0.005" finish cut on the wall which didn't make much of a difference.

Does anyone have any recommendations for machining blocks of aluminum on a router like this and getting a decent finish?  Tooling, feeds, fixturing, I'll take any advice I can get.

Thanks in advance!

[Lee.]

Did you use any oil or mist coolant?

[Marshal]

 Lee., on 20 November 2011 - 01:11 PM, said:

Did you use any oil or mist coolant?

Yeah, I've got a mister setup

[Alvaro Gil - Cimquest-inc.com]

I would try dynamic milling with a full depth cut at 15% step over max. Try the slowest speed on the router. Every time I see one running 20K rpm, I cringe at how much vibration they produce. I'd say keep the chip load at .0005 to start.  Assuming you can do around 8K rpm, that would be 8 in/min with a 2 flt end mill. I bet that's the problem. Also make sure your tool is in there nice and short. How long is the end mill? Try to have it stick out only .25", if the flutes are crazy long buy the shortest one you can that will get the job done. Perhaps post a pic of your setup.

Also, filter the code to make sure it has as few steps as possible. Also make sure the control is in constant cutting mode and not stop mode.

[Marshal]

 Alvaro Gil - Cimquest-inc.com, on 21 November 2011 - 10:38 AM, said:

I would try dynamic milling with a full depth cut at 15% step over max. Try the slowest speed on the router. Every time I see one running 20K rpm, I cringe at how much vibration they produce. I'd say keep the chip load at .0005 to start.  Assuming you can do around 8K rpm, that would be 8 in/min with a 2 flt end mill. I bet that's the problem. Also make sure your tool is in there nice and short. How long is the end mill? Try to have it stick out only .25", if the flutes are crazy long buy the shortest one you can that will get the job done. Perhaps post a pic of your setup.

Also, filter the code to make sure it has as few steps as possible. Also make sure the control is in constant cutting mode and not stop mode.

I don't think I can go much less than about 12k.  

The endmill I was using is relatively long, probably 3/4" flutes or so, although I tried multiple cutters.

I'll have to check on those settings on the control.  I think better geometry might help too, since there's quite a few segments in the quick sample piece I wanted to cut.

[Bruce Kanzelmeyer]

Is the router a 3-axis or 5-axis machine?  I believe that most routers are not rigid enough to allow you to machine aluminum.  We have Thermwoods here and have never had success with aluminum.  They're ok for Renshape or wood, though.

Also, I have better luck with 3 flute cutters when I'm machining aluminum.

[Marshal]

 Bruce Kanzelmeyer, on 21 November 2011 - 01:14 PM, said:

Is the router a 3-axis or 5-axis machine?  I believe that most routers are not rigid enough to allow you to machine aluminum.  We have Thermwoods here and have never had success with aluminum.  They're ok for Renshape or wood, though.

Also, I have better luck with 3 flute cutters when I'm machining aluminum.

3-axis.  The tech for the machine was here last week doing some repairs and he told me people have had plenty of success machining aluminum on their machines, but I neglected to ask him about surface finish or overall quality.  I'm expecting an email from him later this week, so I'll have to ask him then.  I'd imagine the way you hold the piece down would have a big impact on the quality as well, and I just held it down with toe clamps for a quick test.

[Bruce Kanzelmeyer]

What's the horsepower of your router?

[Josh Kinney - ProCNC]

Onsrud 63 Series router bits. I've tried them all in many years of CNC Router cutting Aluminum and nothing beat it, hands down!

https://www.google.c...q=onsrud 63-625

[Marshal]

 Bruce Kanzelmeyer, on 21 November 2011 - 02:01 PM, said:

What's the horsepower of your router?

I think we've got a 5 horsepower spindle on there at the moment.  It had originally shipped with a 10, but that went down a couple weeks ago so the tech came out last week and temporarily swapped it out with the 5.

 Josh Kinney - TMF Inc., on 21 November 2011 - 02:44 PM, said:

Onsrud 63 Series router bits. I've tried them all in many years of CNC Router cutting Aluminum and nothing beat it, hands down!https://www.google.c...q=onsrud 63-625

I'll take a look at those (again).  I think I have a 1/4" onsrud o-flute cutter sitting in my tool drawer, and I know I'd looked into Onsrud cutters previously.

[Josh Kinney - ProCNC]

It has to be the 63 series. It's the only Onsrud that works for Aluminum.

[Marshal]

 Josh Kinney - TMF Inc., on 21 November 2011 - 02:57 PM, said:

It has to be the 63 series. It's the only Onsrud that works for Aluminum.

I have no idea what the brand I have actually is I guess, just a loose cutter that's laying in the drawer.  I'm guessing the ones from McMaster-Carr that are "router bits for aluminum" (McMaster) would probably be the Onsrud cutters, or similar.

[Rotary Ninja]

Do your end mills have any kind of radius? Chipped corners? To finish a pocket floor you need a very sharp end mill. Otherwise the chips will get drug under the tool and cause all kinds of swirls on the floor of the pocket. You see this a lot with radius tools, more often in steel, but in aluminum too especially if your set-up isn't very rigid. Also, a tight helix is best. 45 deg or so. A straight flute end mill side cutting will chatter very badly.

As for the rpm - with that small of a tool I wouldn't see any problem running 20,000+rpm, but you would need a very rigid spindle, and as little tool stick-out as possible. I typically run a 1/8" 2 flute Dataflute endmill at .025" depth of cut, 15,000rpm, and 25-30ipm. Keep in mind this is with flood coolant.

Just curious... how big is the pocket you are cutting? Can it be roughed in with a larger tool?

[Tyler Robertson]

+1 For Dynamic Milling. I get the same results with Robots in Aluminum, and using Dynamic paths made a huuuuge difference