I’m cutting at 16,000 RPM (DeWault on the SO3), 0.015" DOC, 0.04" stepover, and 30 IPM with an 1/8" 2 flute coated end mill. As stated above, I have an SO3 and have never used a Nomad so cannot say how they compare. For me, the above settings yield great results whether I’m adding fluid or cutting dry.
1 Like
Tried again today. Much quieter than yesterday. Not sure it made a difference on the finish of the cut. Settings are as follows:
Result:
This is the 0.125 mill I’m using. Two flute.
The stock is the 1/8" 4x5 sheets from Carbide.
Questions:
-Are the results I’m getting, expected from a 2 flute end mill?. Would a 3 flute end mill make a difference?
-Does the aluminum quality have anything to do with it?.
-Could it be runoff from my machine?.
-Would 10000 rpms make a difference?
Pretty excited with my first experience all in all. It took some time but noise level was very acceptable and being able to do it dry enabled me to use my vacuum system and the was hardly any mess.
2 Likes
@patofoto
The biggest factors in metal machining is a solid Work Hold and a sharp tool.
How are you holding the work?
The Part looks good.
The part seems solid on the bed. Self made clamps to hold while I mill center holes. I then use screws to bolt the piece down using the holes I just milled. The clamps keep holding the stock. This way I can mill the piece without using tabs to keep it in place. The end mill is brand new. @ApolloCrowe, are my results what I should expect from the Nomad at milling aluminum?.
Sounds like a good work hold, the Blue wax is another option to consider.
You have the 883 classic with Belts right?
One thing you could try if you wanted to reduce the small lines seen on the part edge-
Make one final Full-Depth pass at the final dimension, with the previous cuts oversized .003"
What is this part for?
1 Like
Yes. 883 Classic. Like the idea of a finish pass. Will try next. It is a camera tie down. It holds the fluid head to a tripod.
Waiting on the screws from McMaster Carr and some finishing on the wood handle.
3 Likes
The edge you have there looks better. Did you use the exact same endmill, or a fresh one? Take a look at the endmill UNDER MAGNIFICIATION (a 10x loupe is fine) and look for chips or welding.
The exact type of aluminum does make a difference, but the stuff carbide sells is considered “machinable” and should be fine with the feeds+speeds above. The number of flutes will change the engagement per tooth at the same feed rates. I would recommend fewer flutes before more flutes…but it also requires computing the feeds+speeds. 9200 vs 10k rpm isn’t going to make much difference.
You can cut dry, but I wouldn’t try it with an uncoated endmill and expect a great finish. The important thing is to keep the chips out of the cut. I use continuous compressed air for this on my nomad, vacuum doesn’t work well enough.
My (bad) notes to myself say:
.125 end mill, “chinese” - aluminum
Depth 0.0153, stepover 0.035, feed 4.5 in/min, plunge 1.5 in/min
1 Like
@mikep You are right. Slightly better. I did use the exact same endmill. It only had one previous use which was my first aluminum milling that started this post. The endmill I used is coated.
Do you find aluminum chips a problem with moving parts on your Nomad?. You have a compressor for continuous air?. My setup is inside my house and noise is an issue. As it is, the vacuum system is already cutting it close with the wife.
1 Like
So far, no. I’m not running 100psi in there either, it’s enough to clear the cut, but not much more.
Here’s my compressed air setup.
Here’s battle I had with aluminum…
2 Likes
Hi Alek,
This really did come out quite nicely. Are you also using the same alloy as Patricio (6061)? That would be a logical reason for clean vs chattering or even galling when being cut.
Thanks.
Same exact stock from Carbide 3D!
I got a little chatter on my first attempt on these (first time cutting aluminum ever). I tightened the machine up and get the above results. Biggest thing I’ve found is the V wheel tensioning. Mine are set to the tightest setting on all.
1 Like
Nice work all!
QUESTION, 30 IPM at .01 DOC, is this super conservative on a SO3 in one way or the other i.e feed or DOC?
While still remaining accurate ± .008. Thanks Ray
1 Like
I’m finding it to be a bit on the safe side but I’m also cutting 3/4" aluminum all the way through with an 1/8" bit. If my cut depth was a lot less and I didn’t have to have most of the shaft sticking out of the collet, I’m confident that I could cut much faster than the settings above. Pic below is with 30IPM, 0.015" DOC, and 0.04" stepover. Very clean!
3 Likes
I would also like to weigh in here and say that i find using a climb cut for finishing passes produces a nice finish in aluminium (i use 6082 here in the UK)! Conventional cut work well for clearing but climb always gives a nice finish for me!
1 Like
what feeds and speeds do you use?
for 6mm end mills I run at 0.75mm DOC 800mm/min and 290 hertz on my 3 phase spindle (1.5 setting on the dewalt)
for 3mm end mills: 0.4mm DOC 750mm/min (same RPM)
I use more conservative rates as the aluminium available in the UK is 6082 which is a bit harder than 6061 from what I gather.
2 Likes
Added to the wiki, but this points out the advantage the Dewalt has in dialing in an RPM — see Shapeoko CNC Router, Rigid, Accurate, Reliable, and Affordable where I had to note:
16390 RPM (1.5 setting on the Dewalt, between 2.75 (15722.5) and 3 (16870) on a Makita)
What kind of aluminum is that and where do you get it?
This is 3/4" 6061. Got it from a local supplier
1 Like