Working With Aluminum #1

Using a Generic Bit

 

  • Tool: Generic 2 flute 1/8" up spiral bits
  • Stock: 1/16" thick 6061 Aluminum
  • Lubrication: Trend Tool and Bit Cleaner

 

Using smaller tools when working with aluminium can be problematic. Things can go south very fast, then BAM!!!, broken bit.

Sometimes using a smaller tool may be your only choice. This is why I decided to start with a standard 1/8" up spiral bit. These are very common bits and I have used them for everything from polymer clay to aluminum. If you have a CNC, chances are you have these on hand.
If you don't, you can get them cheap here:
Up Spiral 1/8" carbide bits

Note that to use this bit, you will need a 1/8" collet or an 1/4" to 1/8" adapter. I don't like using the adapters as they can add run-out. You can purchase a 1/8" up spiral (up cut) router bit with a 1/4" shank if you don't have a 1/8" collet. I have used this particular bit for several jobs.
1/8" Up Cut Router Bit

I did a lot of experiments with feeds and speeds and started with the following:

DOC=.02
RPM=10000
Feed = 8IPM

DOC=.01
RPM=16000
Feed=16IPM

DOC=.01
RPM=24000
Feed=25IPM

I used a Ramp of .25 with various plunge rates, but found a a plunge rate that is the same as the feed speed worked the best when ramping.

The cuts are done in two operations. The first operation is to make the cut using a conventional cut about .005 shy of your target. The next operation make the same cut but in one operation the whole thickness as a climb cut.

Here is the KRMx02 making a set of holes at the feeds and speeds mentioned above.

I wend one step further and doubled the feed speed.  This would be a more aggressive cut, but the KRMx02 has the rigidity to handle it. 

I used the following settings:

DOC: .01"
RPM: 24000
Feed on Cut: 40IPM, Plunge same as Feed with .25" Ramp
Feed on Finish: 20IPM

I left out the music so you could here how smooth it cut.

This cut is now my starting point with this bit when cutting aluminum.

 

Working With Aluminum #2

Cutting 1/8" Stock

 

  • Tool: Generic 2 flute 1/8" up spiral bits
  • Stock: 1/8" thick 6061 Aluminum
  • Lubrication: Trend Tool and Bit Cleaner

 

Lets take it to the next step and mill something a little more complicated. I will use the last the following settings:

DOC: .01"
RPM: 24000
Cut Feed: 40IPM
Finish Feed 20IPM

Both cut and finish passes use a .25" ramp.

Here, you can see I am gutting a small gear out of the stock using the KRMx02 CNC.

 

This was actually the second attempt at making this gear. In the first attempt the tabs were not strong enough to hold the gear for the finish pass and the gear was ejected (So to speak).

The cause: When my CAM software set the cut shy by .005, this caused a good portion of the cutout in the armpit of the tooth to be left out. IE the curve was a little too tight for the 1/8" bit and the .005 clearance. When the finish cut was made, this section was then cutout at the full depth. No problem, both the machine and the bit can take it but the tabs could not.

In the above video I just increased the thickness of the tabs by about .02 and that solved the problem. If you look at the video during the finish pass, you can see the bit hit each armpit of the tooth. The chips do fly. Did you notice that on the finish pass I did not do a climb cut. This was only because I forgot to change the direction in the CAM software when I created that path. Oh well, it still finished nicely.

FYI, I am sure the armpit between the teeth has a name, I just don't know what it is, and its too late in the evening for me to look it up.