When setting SFM for milling, the feed rate is generally not significant. For milling with the side of the tool, the RPM and the tool diameter determine the SFM.
The actual SFM is slightly reduced when climd cutting, and slightly increased when conventional cutting, but the change is small. At a feed of 2000mm./min (80 inches/min)the change in SFM is 2m/min (7ft/min). With a tool speed of 100m/min (300ft/min), for example a 1/4" tool at 5000RPM, this is only a few percent change, and, in practice, unimportant. At higher speeds, it is less important yet
Tool wear IS an issue, but carbide tooling tends to be quite sharp and stay quite sharp when used appropriately.
With a higher rpm aren’t you just making dust at some point? If you turn the feedrate up with the rpm, you’re still increasing the load on the machine. Why not just increase the depth of cut to dissipate heat better, move more material, and make use of more of the tool?
The struggle is real, to make sense of all the physics and rules and opinions that float around, especially since some of it can be very true on large industrial CNC machines, and not so true on a Shapeoko (rigidity-limited as @PaulAlfaro said)
While I absolutely do not claim to have sorted it out (faaaar from it, I’m still years behind the masters, but they don’t share their secrets easily), I went through the same process of questioning everything, bored people to death here in looong threads about whether chipload matters a lot or not, etc…and then I documented what I felt was a reasonable consensus here. I’m not sure it will make sense to you, but I thought I would mention it. Near the end there is a part about cutting forces and torque and RPM, and a link to @gmack’s excellent spreadsheet that you will definitely want to look into if you are interested in the analytical aspects of determining optimal feeds and speeds for a given situation, on a Shapeoko, with a given router/spindle.
Figure 6.12 of this document shows that the unit horsepower of 7075-T6 aluminum is minimized (to 0.2 HP/cuin/min) with a 2 flute 1 inch diameter endmill at 5000 SFM (19098 RPM). A 1/4 inch endmill would need to spin at 76,394 RPM to achieve that 5000 SFM. That’s likely why these folks and these folks are making high speed air spindles for milling machines.
Cutting power is proportional to cutter speed and torque, and cutting forces are proportional to cutter torque. So, not only does increasing speed improve efficiency, it reduces machine forces.
It all comes down to material properties at temperature, it dictates everything in cutting metal specifically. You want to elevate the temperature of the cut as much as possible because all metals get softer at hotter temperatures. (e.g. blacksmiths) As the cutter moves through the material, the material is being deformed as it turns into a chip, which rapidly increases it’s temperature, making it softer and the cutting easier. In aluminum, you almost can’t cut fast in terms of surface footage of the cutter until you get to really high end machines or use large (+2" diameter) tooling. In various steels, your speed gets limited by the binder in carbide inserts which starts fail at like 1300F if i remember correctly. The purpose of coolant is really to keep the insert cool and not the metal. In nickel based super alloys, the reason those are so terrible to cut is the same reason us humans use them turbomachinery/jet engines/etc; they retain strength well into the temperature range so you end up cutting hard material all the time instead of getting a weaker material locally as the chip forms. This is the reason ceramic tooling became a thing; unlike carbide that breaks down at ~1300F, ceramic doesn’t care about anything until like 3,000F at which point anything metallic is probably a liquid.
Think about things in terms of metals getting weaker as they get hotter balanced against how carbide breaks down and you’ll understand why all these metals have different surface footage requirements.
If you can cut something or cut something half as strong, pick the less strong thing…up to the point your tooling gets too hot and gets weak as well.
My aluminum real world experience cause these guys already geeked out lots of good information
More RPM more MRR. Tool life isn’t much a concern for us as we generally dont push tools to its limits. Single flutes love rpm and match very well with hobby machines. My S3 has run from 8,000-60,000 rpm (world’s fastest? Lol). The MRR with 1/8 tooling was higher than some 1/4 stuff ide run at 30,000 lol.
Everything matters and as the rpm goes up, certain things will matter more. Chip clearing, helix angle, heat input, heat management, chipload, tool balance, feed speeds, accelerations and feed optimizations.
Ohhhh and sometimes you can “outrun” chatter. It’s a vibration thing.
1.2kw wasn’t quite enough. Water cooled was a hassle because that sucker produced a ton of heat.
Running an air cooled 110v 80mm 1.5kw with good results and more than enough tq now. Boring, but running dry without airblast its usually better to stay lower rpm anyway.
We discussed the concept of SFM in an earlier post I last year. The consensus we came to and that I agree with upon further review is that SFM doesn’t really matter for CNC router milling. The origins of SFM came about with perhaps roots in thermal heat generation and metal melting points but no one has a good story and they don’t seem to matter. What matters more is the chipload, as that is proportional to the heat generated since that is how much material you are removing per cut. With CNC companies like Datron, PocketNC, and Kern milling aluminum on 50k spindles, we can certainly do it with 30k routers.
The only thing to be aware of is that at higher SFMs, you do generate more heat and misting some IPA/H2O helps alleviate that and provide lubrication to evacuate chips more effectively.
SFM is optimal material removal rate for best possible finish. Cutting metals at all on a tabletop CNC router means breaking all the rules though, because the machines are flexible and don’t have a lot of inertia/mass to dampen vibration or keep from chattering to extremes. High RPM kinda just cheats this away but isn’t optimal for most ideal material’s SFM.
Yup - that’s why high cutting speeds (RPM/SFM) are so helpful for CNC Routers. They help mitigate the impact of the lack of machine rigidity and feed force. What is the “most ideal material’s SFM”?
As @Vince.Fab and others here and elsewhere have demonstrated, high speed machining (HSM) techniques can provide significant increases in the capability of CNC routers, including Shapeokos and Nomads because of the cutting force reductions they enable.
An explaination of why HSM works (as of 1977) from page 16 of the Handbook of High-Speed Machining Technology:, "Almost all of the energy of metal cutting is used for plastic deforming of the chips and in overcoming friction between chip, tool, and workpiece. All of these actions result in heat, and that fraction dissipated in the tool causes softening and reduced resistance to abrasion, thus limiting tool life. Consequently, the crux of the problem of super-high-speed machining is to concentrate the heat in the chips and minimize the quantity of heat transfer to the tool.
It is postulated that the heat generated per unit volume of metal removed should be lower at very high speeds because ductility of metal decreases with increasing strain rates. In addition, if the heat accompanying deformation is confined to the chips, chip temperatures will be raised and their strength reduced. Unfortunately, the available data do not permit quantitative estimates of importance of temperature and strain rate on the energies required for deforming chips at excessively high speeds.
In addition to the points discussed, high-speed metal cutting seems feasible on other grounds. It might reasonably be expected that the tool would not reach a high temperature, even when the heat liberated in the chip is higher per unit of time, because the time available for conduction is limited by the high speed…"
All of this is really interesting, thanks for putting so much into this post. You guys have brought out some great information.
I find this piece of info on high speed machining especially interesting. I’m very curious on what I see missing in this explanation. When a chip is cut and it leaves with thermal energy imparted on it. Yes that makes sense but what about the heat imparted on the cutter and the piece?
I can guess that the chip is heated by the deformation it experiences while being cut (as how the chip comes out bent), but I have to be curious about the other sources of heat, and how those affect the work piece and cutter. Thermal conduction is bound to happen between all points of contact, but due to the high speeds I doubt this is a major contributor to heat in any of these elements (i’m looking into it though. please).
Also of people have talked about heat generated due to the rubbing that happens between the cutter and work piece as a major contributor, and my intuition seems to agree with this. Since the cutter isn’t infinitely sharp there’s bound to be aluminum left on the wall as the cutting edge passes along it, and that I’d guess bounces back and rubs against the rest of the cutter beyond the cutting edge. That’d create heat as well as deflection. I looked a bit at an end mill and I noticed there’s a slice along the side of each flute, and I’m guessing this is to reduce friction. However it doesn’t get rid of all of the side, so there’s still some contact.
A friend of mine pointed out that energy is also released when the metallic bonds are broken, but I’m still figuring out how to calculate that cuz that means somehow calculating how many atomic bonds are broken when a chip is cut.
Yeah so if you didn’t feel like reading that, what are the sources of heat that heat the cutter and work piece in a cut?
There is another very long thread about these topics that you shouldn’t miss. I think you’ll be interested in it. It starts out a little slow, but the conclusions are a blockbuster!
