Aluminum Feeds, Speeds, and Depth

[adam....@gmail.com]

Hi,

I'm trying to make my first part on the PocketNC (original model, new spindle). I'm making the part out of aluminum 6061. The first cut is to make a large hole (2.375" diameter, 0.6" depth) in the block.

I chose to use the largest diameter tool that would work with the spindle (5/16"), and worked with the Feeds & Speeds tutorial ( http://www.pocketnc.com/feeds-and-speeds ) to figure out the various parameters.

If I'm reading the tutorial correctly, here's the values that I should be using:

-Speed: 8500 RPM
-Feed (using a 2 tooth tool): 0.0008 * 2 * 8500 = 13.6 IPM
-Side Load: 10% * 0.3125" = 0.03125" --> this goes in the "maximum stepover" field in Inventor HSM
-Depth of cut: 90% * 0.3125" = 0.28125"

I tried this and it was very apparent that the spindle couldn't handle this load. It would get stuck very quickly while ramping into the metal. I tried cutting the depth in half down to 0.14" and it failed again. I tried cutting the depth in half again down to 0.07" and it failed again. I cut it down to 0.04" and it is working now, although to the moderatly-trained ear, it sounds like it is right on the edge of struggling.

At this rate, it's going to take me a roughly 4 hours to make that hole. That feels like an awfully long time to make that hole, but that might be the limitations of this machine.

Also of interest: I used the "feed override" bar in the GUI to pump up the feed rate to 150% (ie, 20.4 ipm) and it seems to be working fine, so that's a positive note.

Am I thinking about this right, or is there something I'm missing?

One other point of interest: At times, my PocketNC doesn't turn on properly. I'm not sure why. I flip the power switch on, and I can see some blue lights behind the HDMI port, but not the several blue lights that you can normally see when the power is on. I've haven't figured out the pattern yet as to when it will work or not. I suppose there is some power problem which might explain both issues (not much power to the spindle, and also not enough power to the Beagleboard sometimes), but I don't really have any evidence to confirm that.

I appreciate any thoughts on these issues!

-Adam

[Michael]

Adam,

As far as the BeagleBone is concerned. I would make sure the machine is fully turned off before trying to turn it back on. Think of the machine like a USB device. If you disconnect from a USB device it will not allow the computer to reconnect until the device has been fully powered off or disconnected. The BeagleBone will not power back on until it has fully powered off. If you leave the BeagleBone main power on or leave the machine connected via USB the machine will not fully power off. This is one possibility of what could be causing the machine to act up when you try to power it on. The solution is to shutoff the main power and unplug the USB connection to the machine for at least 1 minute and then try to restart the machine. Let me know if this doesn't work and we can go from there.

When looking at the feed rates and cutting on the machine I would recommend using a 15% stepdown and a 60% step over. The 15% stepdown allows for a lighter cut resulting in better feed rates. The 60% stepover results in the tool getting more engagement into the material creating a smoother cut. The numbers we give online are general rules of thumb that may not always work well. I will look at them again and adjust them accordingly. We have found a small stepdown and large step over to work well in most applications.

The other thing to think about when machining, especially metals, is the spindle torque will drive the allowable tool diameter. When cutting aluminium you will have better results using a 1/8" endmill. The smaller diameter will allow you to cut more effectively with the spindle torque provided. 

Let me know how things go. A lot of the machining process is tinkering with the settings until you find the sweet spot for the tooling, material and cutting process you are using. 

Have a great day,

Michael

[mic...@cyto365.com]

This is my settings for aluminum, 6mm 4 Flute endmill, 10 000rpm, stepdown 0.25mm, stepover 5.7mm, feed 400mm/min.

Since we are limited to 10 000rpm, we can only increase by increasing number of flutes. Then I believe the other fixed value is step over that seems fine at 5.7 mm as suggested by fusion360. What is left is to balance stepdown with feed.

For the last finishing strategy I use only 0.05mm stepdown and 100 mm/min Feed. Then I get a really smooth surface for e.g. face operations.

Best regards

Micael