There’s not a lot of threads about feedrates and cutter speeds yet, but it sounds like the 8-16ips @5000-10000rpm 0.01DOC in aluminum seems to be at least working for people.
Looking at carbide create’s defaults for aluminum I get some weird numbers.
for 1/16, 1/8, and 1/4 end mills it recommends 9000RPM for them all and feed rates of 13, 36, and 18 IPS respectively. the 36 IPM seems a bit fast relative to what I read people here using. Does anyone cut that fast?
I did try 12(@10krpm), 16, and 24 IPM. For me 12 IPM was the worst. It was VERY noisy/chattery. 16 sounded pretty good and 24 was a bit loud but not too bad. They all had comparable surface finishes.
Me, I never use C3D numbers. I do them myself, starting with G-Wizard recommendations. I factor in deflection so my rates tend to be lower than some but I get a great finish.
I rough 6061T6 on the Nomad @ 20 IPM, 10K RPM using 2 flute, ZrN/TiB2 coated end mills. The Nomad cannot use 0.25" end mills effectively for metals. I don’t even suggest trying.
End mill materials, coatings and helix angles matter:
Please provide some details and we can provide some guidance.
I did try 12(@10krpm), 16, and 24 IPM. For me 12 IPM was the worst. It was VERY noisy/chattery.
Feeds and speeds has a solid basis in physics and mathematics. The feed rate and RPM must be coupled properly for the available spindle torque to obtain a clean and optimal result. Too slow a feed and the end mill may not be cutting anything… until a step occurs… and you get a racket.
Adding in deflection to the equations ensures that secondary and tertiary effects do not create problems… and tool life is improved.
Sorry I’m using the 1/8" two flute endmill that came with my Nomad 883 pro. They’re uncoated. I’m cutting 6061 (not sure if it’s -T6). I’m very willing to buy different cutters if it’ll get better results. especially faster roughing. I’m also willing to change alloy.
After my test cuts and plugging in the values to a SFM and chipload calculator my next test was going to be 10krpm 20IPM so it sounds like that’s a good combination. What depth of cut do you use? Do you recommend any specific end mills?
EDIT: Oh, also do you have any recommend settings for a finishing pass? Specifically for getting the best top surface quality?
Sorry I’m using the 1/8" two flute endmill that came with my Nomad 883 pro. They’re uncoated.
NOW WE’RE GETTING SOMEWHERE!
I’m cutting 6061 (not sure if it’s -T6).
The most common variants all machine similarly. Let’s ignore this for now. In general, one needs to know the specifics of the metal they are machining. My 6061 is 6061-T6511 (the 511 is getting super specific; not pertinent to this issue). Better to know than to not know… knowing allows for optimizations.
I’m very willing to buy different cutters if it’ll get better results. especially faster roughing.
ZrN or TiB2 will allow modest improvements in speeds and will increase the life of the end mill. Well worth the extra expense. C3D stuff is pretty good… but one can do a fair amount better. More below.
I’m also willing to change alloy.
No need. 6061 is awesome. In the future, for general work, T6 is an excellent choice. T6 is very common so I wouldn’t be surprised that you have it. I would stay away from T1 until you’ve got some experience - and need it.
After my test cuts and plugging in the values to a SFM and chipload calculator my next test was going to be 10krpm 20IPM so it sounds like that’s a good combination.
Yes, that sounds good.
Do you recommend any specific end mills?
Read my posting… I mentioned it above… it’s all there!
Before you order PM me and we cover the details.
What depth of cut do you use?
0.04. I would try 0.02 for your current tools. If you like that, try 0.03. Coatings get one extra distance.
Do you have any recommend settings for a finishing pass? Specifically for getting the best top surface quality?
Mark has pretty much covered it but I can add something to this.
All I cut is Alu,mainly T6,I use a combination of a 3mm 2flute 45 Helix cutter at 16000-17000 Rpm with a .17mm DoP with a feed of 400mm/min,Alu I find favours a thin and fast approach rather than the Ron Jeremy Deep and Slow,I finish with about 200-250 mm/min,similar to Marks approach.
It also depends on what you are asking it to do,I do a lot of thin panel work so my technique is focused towards that,I have to work around panel lift as the center of the stock is normally unfixed and can be lifted by cutter action.
Also worth pointing out that cutter diameter is crucial to material removal and ejection which is directly linked to the cut speeds you can attain,the larger the better.
I’ve been cutting 6061-T6 on my Nomad 883 Pro with Lakeshore Carbide 1/8’’ two flute ZrN endmill with a feedrate of 12ipm @8000rpm and a 0.01in DOC. It is sometimes very loud (especially in some directions weirdly). So it seems like I am going too slow according to your recommendation.
What DOC are you using for this feedrate? You mentioned 0.04. If so I seem to be going really slow.
Will it be a good idea to have a thread for feedrates? I think it will help a lot for people who are new to CNC. I have made mistakes and broke cutters (1/32’’) when I went too fast and it seems I am going too slow now.
Thank you for your help! I am planning to cut Aluminum this weekend and I would love to be able to go faster.