Aluminum tips?

Thanks Ryan,
20 mm/s feed rate
.2mm/s plunge
3 mm doc
12,000rpm
1/8 double flute endmill

Trochoidal
2% step length
50% width
.05mm oscillation

I feel I can easily up the feed rate without issues, I may try 30 mm/s. but I’m happy with 20 mm/s, giving the size of my machine.

I think 20 is pretty fast I would stick with that and increase your depth or step length instead. If you feel the need to push it harder.

The part looks great. I’d be happy if I cut that!

1 Like

Looking great Mark. Those are some nice cuts. The guys are giving you some great advice. Remember when cutting metal its not always about the speed of the bit, its about torque and the amount of metal your bit can effectively clean away with each pass. The chatter you were getting earlier can result from a few things. The main factors in my mind are load on the bit, horizontal in this case, and the speed or effective cut of the bit. And in some cases harmonics depending on how well the material is fastened to the table and if it is reverberating or not. Looked like it was held down pretty well so harmonics is the least likely. The Trochoidal seems to be the way to go with these machines as the guys suggested above. Keep playing with the settings and let us know what works. You also might try a single flute bit as Christian suggested above. It’s a juggling act between speed and torque of the spindle and the effective material removal of the bit at those given rates. I plan to have my MPCNC built in the next few months and will be trying some aluminum as well even though the primary use for the machine will be wood.

1 Like

Thanks for the reply Johnny.
Thanks for the advice, the guys here have been a big help as well.

Each time I turn my machine on and cut aluminum it’s getting better, tweaking and adjusting as I learn. Just did two more parts. Trochoidal is working very well for me. I’m going to order some single flute bits to try out.

IMG_5917.jpg

Very nice! Cuts are looking really good. Im excited to see how you progress. Once the 3d printer gets here I be getting started on my mpcnc as well. Most of my cnc background comes from running lathes instead of mills, but cutting chips translates some from method to method. Let us know how that single flute works. Speaking of I saw a video from a tool company on YouTube specifically about Trochoidal. The make bits specifically for that style of cutting and use what looked like a 5 tooth or flute bit. But its for larger machines mostly. Very interesting cutting method that I am interested to explore myself.

1 Like

Very interesting topic, congratulations on your results!
I really want to try that soon!

1 Like

Jonny I seen a video too on the trochoidal bits but didn’t see on their website where to order them, would be interesting to try out.

Thanks Dui, I really like your build!

Trochoidal is a milling strategy that works with any bit but generally is used with a square endmill.

For those using Fusion 360, I believe they call this ‘adaptive’ milling

A little different but the milling strategy I think most beginners should start with, and this video has a really clear explanation of it. https://youtu.be/_N5VaTchhys

I think this is a little closer to the “peel” in estlcam. I am not positive but I think the strength of Tricoidal is in using it on a single cutout type path So you get a constant load of half the bit instead of climb and conventional milling at the same time, where peel and adaptive are clearing strategies. Again I am not 100% on this.

Ryan,
There’s a company that’s making speciality bits that takes advantage of trochoidal milling method. Think it’s a German company, need to see if I can find the link again. Wouldn’t mind trying one.

Hi,

single flute is IMO the most reliabe option for hobbyist purposes in aluminum.
It is just the most tolerant tool as the range of feeds and speeds actually working without breaking the tool is comparably large.
There are special tools for trochoidal milling - but their focus is usually to maximize material removal rates - not best possible tolerance of different machining conditions.

I’ve experimented with different tools in the past but now only use single flute for aluminum.

Not a MPCNC - but some aluminum milling with Estlcam and single flute tools:

[youtube]http://www.youtube.com/watch?v=U7yn399bE1I[/youtube]
[youtube]http://www.youtube.com/watch?v=HxkKXm55UJY[/youtube]

Christian

4 Likes

Hi Mark,

 

How long it took to make the part? When I use estlcam it calculates will take aproximately 18 hours for a part 400mmx400mm with throcoidal milling.

Manuel,

Sorry for the delay, thought I replied.

I find that my run time is way longer then estlcam and repetier host shows. Maybe 4x the time it shows.

I just finished a large part 20" x 20" (508mm x 508mm). Just the outside cut took about 36 hours.

Just finished milling out this part here 20"x20". Broke the job up over nights and weekends. Need to sand, clean up my mistakes then powder coat.

Mark, what bit and settings did you use and how thick is that? It is an amazing job but those cut times are way too long.

Ryan,

its 1/4" thick. I used a 1/8 double flute endmill.

trochoidal milling, 2.70mm doc, 30mm/s, 2.0% step over. I feel I could have went deeper or raised the step over. For the holes I used a 1/16" endmill. I did try a single flute endmill but within less then 5 minutes I broke it… oops

One thing I do notice with trochoidal is that when the jobs done, when it goes to return to the zero spot that it’s about 3mm forward in both x and y. I don’t see that when doing convention milling.

Kevin’s settings see to be pretty good. Swinging the router around at 30mm/s might cause you to skip steps if you are running it 8hrs at a time.

Give his settings a try.

1 Like

Thanks Ryan,

I’ll give those settings a try. I should be back to milling aluminum in the next few weeks. Going to have a little fun with wood and pvc board.

Apologizes for necromancing this thread but is there a reason you guys aren’t using any cutting lubricant?