CNC Aluminum: Recommended Speeds/Bits?

[mrnoble]

We've had limited success using our CNC router with aluminum. Anyone have recommended settings for pass speed and spindle speed, as well as recommended cutter types? Thanks!

[techhelpbb]

It really does matter what exactly your CNC router is...but....

Single flute and you can go move fast as long as you balance that speed with: the proper spindle speed, cut depth and machine rigidity.

There are speeds and feeds calculators and charts.
I do not want to recommend a specific speed because you did not provide enough information to understand the implications.

[rcoren22]

We just got a CNC Router this past Sept and started cutting Aluminum with some success starting last week.

Last night we made custom drivetrain plates from 3/16" 6061 Aluminum.

We have been using a 5/16th end mill while waiting for our shipment of

Onsrud
G1817076 Upcut Spiral O-Flute
and
G3168471 Straight O-Flute bits.

Spindle Speed - 10,000 RPM
Feed Rate - 20 IPM
Plunge Rate - 10 IPM

*Make sure you have coolant. We are using a spray system with a vegetable base spray.



Let me know if you need anything else and good luck

[techhelpbb]

Originally Posted by rcoren22

Let me know if you need anything else and good luck

What machine do you have?

[rcoren22]

Originally Posted by techhelpbb

What machine do you have?

We got a Camaster Stinger 2.
1.7 HP HSD Spindle
900 oz- Nema motors
Mister System
Phenolic Top
Couple of other goodies.

[JamesCH95]

Step 0 with any CNC machine (IMO): get GWizard. Life will suck WAY less. It even has rigidity models, which will help guide your feeds and speeds by de-rating power on less-rigid machines like routers.

Here is a blog entry from the guy that makes GWizard. Worth a read. Then a re-read. Then another re-read after you try some of the suggestions.

http://blog.cnccookbook.com/2012/03/...tting-success/

Originally Posted by Ronnie314

Is that running on 110 or 220? We are looking for something to do precise machining on our aluminum and only have access to 110.
-Ronnie

110 is more than enough for a capable router table. My 4x4 Small Shop Machine is 110 and I've had good results cutting aluminum.

Originally Posted by mrnoble

Also, we have no coolant. Which could be a problem, but it's primary use is wood and plastics, and with the vacuum table I really don't know how we'd make a coolant delivery/extraction system work.

Are you at least running a serious air blast to make sure chips are not being re-cut? If neither of these then I think I know your problem...

[MichaelBick]

GWizard is useful. Otherwise you can look up how to do feedrate and spindle speed calculations online.

As far as what you need, you're going to want a 1/4" single flute onsrud end mill. You also want a mister.

This thread is great.

[Jared]

As others have said, Onsrud bits are the way to go. We use a .125" single flute end mill designed for cutting aluminum, and we can go about 100 ipm comfortably through .125" aluminum.

We haven't had much luck with our vacuum table as a reliable hold down. Instead, we like to use a combination of double sided tape and clamps on the edges of the material.

The mister has a tendency to saturate the air in your shop with coolant, which smells strange, and probably isn't very good for long term exposure, so we've just had somebody with a spray bottle spraying some coolant (mobilcut 102) ahead of the bit.

To clear chips, we've just zip tied an air line to the side of the spindle that points right where the cutter enters the part.

[Mr. Lim]

Highly recommend the Onsrud single-flute cutters as well. We use them religiously in our lab on our CNC router. We run .125" to .250" diameter cutters depending on the parts

We use a Unist mister and coolant setup on our router, and are very happy with it. It periodically deposits a mist of coolant, and it doesn't seem like very much of it aerates. I don't ever smell it. I haven't noticed any changes to the environment/air since using them. We run 4 of the mister units in a very small workshop on our lathe, cold saw, manual mill, CNC router. All the mist seems to end up on the workpiece and machine (not in the air), and clean-up is a simple wipe down.

[Bruceb]

Why do you use both up spiral and straight bits?

[JamesCH95]

Originally Posted by Bruceb

Why do you use both up spiral and straight bits?

Spiral bits are used for extracting chips from the cutting area. This is great for contouring holes, slots, pockets, and other features where chips tend to build up.

Straight bits, also called edging bits, won't extra chips as efficiently (or at all) but they also won't lift up on the part they're cutting. This makes them useful for trimming the edges of parts as there is plenty of room for the chips to go and they don't lift up on the part's edge, potentially causing chatter.

[Andy Brockway]

I have a really old CNC router with a standard wood router running at 30,000 rpm. I have had success cutting aluminum with an 1/8" diam straight router bit at 10 ipm, .005 DOC. This is slow but I do not run coolant and it does not clog the bit.

[mrnoble]

Sorry, we have a Techno Isel 31" x 33" Servo Gantry with a 5HP 6000-18000 router. We also have the vacuum table setup.

[techhelpbb]

Originally Posted by mrnoble

Sorry, we have a Techno Isel 31" x 33" Servo Gantry with a 5HP 6000-18000 router. We also have the vacuum table setup.

Going to see if I can figure out how fast your Techno Isel can move the table axis around. If you know it would save me the effort. The fact you have a servo drive pretty much removes the top end speed that would likely exist with stepper drives.

What problem are you having cutting aluminum:
Deflection?
Chip welding?
Stalling?

[RonnieS]

Originally Posted by mrnoble

Sorry, we have a Techno Isel 31" x 33" Servo Gantry with a 5HP 6000-18000 router. We also have the vacuum table setup.

Is that running on 110 or 220? We are looking for something to do precise machining on our aluminum and only have access to 110.
-Ronnie