Cutting Aluminum Experiment

[joewino]

This morning I was experimenting with cutting aluminum. We've used the ShopBot for a lot of MDO and HDU but have received requests for cutting aluminum for push through letters.

My test piece was an .040 aluminum sign blank. The bit was an Onsrud 64-012 - 1/8" downward spiral.

I was experimenting with feed rates and RPM and could never get to the point where there was not a lot of burr on one side of the cut.

Also, I started out at a Z depth of .039 and it cut only about half way into the aluminum. As I changed feed rates I found that there was less burr on one side, but the opposite side of the cut was still messy. In addition, with each trial I set the Z depth deeper and deeper, but it would never cut through the aluminum.

My final cut was at .06" (15,000 RPM - 40 IPM) and the bit broke.

The only cooling was the dust collector moving air and some WD-40 sprayed on the bit.

I've also experimented with some .080 with similar results, other than breaking the bit. On the .080 I was using a 1/4" bit but was still getting a lot of burrs and could never cut all the way through the material.

No vacuum - material held in place with double stick tape.

Any ideas?

[David Iannone]

Ray,
I have cut aluminum in the past. I use the onsrud bit 1/8" UPCUT SPIRAL O FLUTE ONS63-712. I have a porter cable and was at 16,000 rpm I think with a move speed of .5 ips. I have a PRT Standard. I got a nice cut on both sides.

[gamisano]

WATERJET! I had same issues cutting di-bond, which is aluminum sheeting with a plastic core. I used the special 45 degree bit that onsrud sells, and could not get passed major aluminum building up on the sides. Maybe my standard PRT was too slow, or something. Alas, I took it to a local waterjet guy who cut what I needed in ten minutes with beautifully clean edges. well worth the $100 minimum he charges.

Guido

[Brady Watson]

Vacuum hold-down is pretty much essential for cutting AL sheet. DS Tape isn't going to work very well and it gums the cutter.

You can use a standard end-mill and get great results. Start by trying a 1/4" diameter tool with the SHORTEST cutting length you can get. The longer it is, the more it vibrates and degrades the cut. If the AL sheet is vibrating because of inadequate hold down, then this will contribute to bits breaking and poor cuts. Down cuts don't usually work very well on AL in my experience.

With a 1/4" end mill (like a spiral upcut), solid carbide & short cutting length, you should be in the 13,000 to 16,000 RPM range and running between 1 and 2 IPS. Use small diameter cutters sparingly. Save your cash and use end mills...they are afterall what we use to cut AL on a milling machine. If you go too slow, you are going to heat up the bit and it is going to break...too fast & you overload it & it breaks - most likely because it is too long.

Learn to 'listen' to what the machine is telling you. Measure the chips coming off of the cutter. Check against chipload calculator in SB3 under tools. This is not an absolute, just get into the ballpark to start, then adjust for YOUR machine. You want the biggest chips you can get without overloading the bit, while maintaining a nice edge quality. Bring the move speed up a little higher than you think it should be & adjust RPM and/or move speed on the fly as you are cutting. Observe what is going on & you will find the sweet spot.

Waterjet not required...listen to what the tool is telling you and you will learn to cut darn near anything. I have consulted a few shops on cutting AL sheet (all they do) and Dibond with excellent results...don't give up, keep trying!

-Brady

[joewino]

Thanks for the advice. I will continue to experiment, using your information.

Why wouldn't the bit go all the way through the aluminum?

And how do you adjust the RPM and move speeds on the fly?

[Brady Watson]

1. Set your Z speed to .1 or .2 IPS. Keep a short safe Z height so it doesn't take forever to get to the surface of your material. My guess is that you are plunging too quickly into the material & the Z axis is stalling & not going all the way thru. Another possibility could be that if you are using foam tape, the material is squashing down enough to keep the tool from applying enough force to pierce the material.

2. Adjust move speed via Shift and '<' or '>' keys on the fly. Be reasonable with how much you increase the speed since it doesn't recalculate ramping. Change router speeds via your VFD or your RPM slider on the router itself if yours is setup that way.

-B