# CNC Routing Aluminum Face Plates - Need Help



## Mahonroy (Jun 2, 2015)

Hey guys,
I am creating aluminum face plates for a device I am building, and I am doing this with a CNC routing machine (using 1/8" shaft sized bits). Here are some photos of what the face plates look like:









































It has been a challenging task to get the machine set up to cut out the various shapes/pockets, and its still not working correctly and is definitely not a reliable process. My problem is that I keep breaking bits, so initially I started slowing everything down, and the bits would stop breaking, but it would then start generating a lot more heat and the cuts didn't look very clean. This also added a lot of machining time to it, and still periodically bits break.

Here is some info on my machine.
I am using a Chinese 3040 CNC routing machine that I have upgraded. I swapped the stepper motors and controller over to the Gecko g540, and upgraded the spindle to a 450 watt, 10,000 RPM spindle. The machine seems to be solid and well built. I also have an RPM reader on the spindle. I am also using "Cut 2D" software to generate GCODE.

The cuts that are giving me the most trouble are the 0.125 end mills, and the 0.0394 end mills. For the 0.125, my pass depth is 0.01", and feed rate was 8" per minute. Everything is 10,000 RPM. I was using a single flute HSS end mill. This worked alright, but was slow, generated a ton of heat, and the cut was not clean at all (lots of melted metal looking burrs everywhere), but the bit rarely would break. I then tried switching over to a double-flute bit, and it seemed to work better. I then tried using some speed/feed calculators and found that I should try a faster feed rate; so I tried 14" per minute and it appeared to be cutting great.

The problem is that after a while, little aluminum bits start to build up in the cutter, and everything starts to get hot, and then the bit breaks. I am averaging 2 face-plates before this starts to happen then the bit breaks. I also wanted to note that the RPM's stay right around 10,000 RPM, it doesn't really slow down once its cutting.

Here are a couple pics showing the jig setup... and notice how the cuts start out fine, but then quickly goes down hill by the 3rd and 4th plate. Also note, that total cut depth is 0.06" deep, so this is 5 passes:

















I recently ordered a couple of 4 flute bits to experiment with... but honestly I just don't know... seems like I just don't know whats going on and figured I would ask you guys. I am also tempted to try and reduce the pass depth even more (from 0.01" to like 0.005")... but that's already a really small bite out of the metal and it seems like it should be able to handle this better?

Anyways, any help is greatly appreciated, thanks!


----------



## subtleaccents (Nov 5, 2011)

I think your 10,000 RPM is slow for the .125" bit. I would change up to 16,000 to 18,000 RPM. Your feed could run closer to 18 to 20 ipm for starters.
A small amount of kerosene applied with a small brush will help prevent chip build up. Are you using a router bit or a end mill?


----------



## Mahonroy (Jun 2, 2015)

subtleaccents said:


> I think your 10,000 RPM is slow for the .125" bit. I would change up to 16,000 to 18,000 RPM. Your feed could run closer to 18 to 20 ipm for starters.
> A small amount of kerosene applied with a small brush will help prevent chip build up. Are you using a router bit or a end mill?


Thanks a lot for the reply! So I heard that if using a single flute mill bit, that I want closer to 20,000 RPM, and a dual flute mill bit closer to 10,000 RPM.... do you still think I should go higher RPM and faster feed speeds?

I have never used a cutting fluid, so I will definitely try it. I was originally worried that the fluid would make a mess, would mess the jig up, and would stain the anodized plating... but maybe if I find the right one (or use ethanol) then I might be ok?

And its an end mill bit, it looks kinda like this:









And this is what the single flute one looks like (the one I used to use)


----------



## Shadowrider (Apr 1, 2015)

Definitely too slow. I'd run that spindle 30,000 if I could.

Don't know if you can find any bits like this but for high speed machining of aluminum in the aerospace industry we used 3 flute bits a lot. Stiffer than 2 flute but not near as prone to chip clogging of the flutes as 4 flutes. If you go with 4 flute they will be stiffer by a lot but be prepared to turn down the feed rate some due to chip clogging. Carbide is your friend for it's increased stiffness. Ditto on the kero too, even water will help.


----------



## fixtureman (Jul 5, 2012)

I was told that a hss bit is better for aluminum as it is not as brittle. and lower speeds and feeds like when they mill on a milling machine.


----------



## Stick486 (Jan 4, 2013)

waxing the bit helps...


----------



## Dr Neon (Apr 15, 2010)

What grade of aluminum are you using? Too soft (~3000 series) and you will gum up, and ultimately break, any bit.
5000 or higher series aluminum is harder, and chips better (especially at higher rpm's). I would use a carbide bit, higher
grade aluminum, and higher bit speed. Should be no need for coolants. Worked for me. (large sign letter cut-outs).


----------



## subtleaccents (Nov 5, 2011)

Mahonroy said:


> Thanks a lot for the reply! So I heard that if using a single flute mill bit, that I want closer to 20,000 RPM, and a dual flute mill bit closer to 10,000 RPM.... do you still think I should go higher RPM and faster feed speeds?
> 
> I have never used a cutting fluid, so I will definitely try it. I was originally worried that the fluid would make a mess, would mess the jig up, and would stain the anodized plating... but maybe if I find the right one (or use ethanol) then I might be ok?
> 
> ...


If you are worried about messing the jig or the surrounding area with a cutting solution you can use corrugated sheet, like a box and cover the outside area of the part being cut. I have done this and it works very well. Just throw it away when you are done.
Remember, we are not talking about flood coolant, just a small amount to keep the bit lubricated. I never tried ethanol. It may have a evaporation rate too quick to be helpful without applying a large amount.


----------



## Mahonroy (Jun 2, 2015)

Thanks a lot for the advice! I ordered some 3 flute end mills (they have not arrived yet), but did some calculations and found that for my 10,000 RPM, 2 flute, 1/8" end mill I should be closer to 20" per minute. So I changed it from 14 to 17. I also added some compressed air to blow away the chips, and between these 2 things its looking pretty good. I think with the 3 flute end mill it will be even better.


----------



## SteveMI (May 29, 2011)

DrNeon said:


> What grade of aluminum are you using? Too soft (~3000 series) and you will gum up, and ultimately break, any bit. 5000 or higher series aluminum is harder, and chips better (especially at higher rpm's). I would use a carbide bit, higher
> grade aluminum, and higher bit speed. Should be no need for coolants. Worked for me. (large sign letter cut-outs).


I tried 3000 series aluminum a while back and had the gum / break problem. Also the end result looked poor.

With the 6061 grade, the same bits worked fine. I found that aluminum is a bit like plastic, you need to have a feed rate that produces chips and doesn't allow the aluminum to melt.

Steve.


----------

