Usual preface, I’m with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.
So… This might be more than you are currently looking for. But I’ll try to give some basics on how this all work.
The first thing I would say is throw “feed and speed” out the window. It’s not really what matters but rather a “short cut” to get to what really matters. The things that really matter in this are chipload and surface speed. Chipload is probably the most important factor in milling overall and is required to understand a lot of the other factors. So I guess let’s start there.
In simple terms chipload is the “width” of the chip you are cutting per flute per rotation. Or a sometimes easier way to think of it is it’s the amount the CNC is moving “forward” (in X/Y) per flute per rotation. The reason it’s so important is that there’s a minimum chipload per material and tool combination that you have to hit to not “rub” (using the tool as glorified sandpaper and generating a ton of extra heat and cutting forces). While at the same time it’s also one of the 3 factors that are responsible for cutting forces that the tool, CNC, and material have to resist. You’ve already seen some effects of this by burning the wood. Too little chipload = too high of heat.
Surface speed is the rotational velocity of the edge of cutter. There’s a lot of wiggle room in things like wood for it. In general though the higher the surface speed the higher the searing force for the same cutter. However, you can get to a point where the surface speed get too high for the material. This will damage both the tool and material regardless of the chipload (feed).
I should probably also talk about cutting forces here. The machine, tool, and material have to resist the cutting forces. they increase with the cubic material removed per flute. So the stepover, chipload, and pass depth all proportionally increase the cutting forces. Though not always in the same direction. You will get different artifacts in your cut depending on which you exceed. If it the material it will start to rip material out instead of cut. If it’s the tool or machine it will typically “bend” out of the intended cut path. Eventually enough of any of those will break the tools as it radically changes the the functional chipload or just straight bend the tool to the breaking point.
So with those out of the way, how do we actually calculate a usable chipload and surface speed? It’s complicated… At a fundamental level what we need is a chipload that is “cutting”, a surface speed that is under the damaging point, and cutting forces that are within our tolerance for the machine, tool, and material. These are also all effected by other factors like tool geometry, runout, and acceleration. There are some “rules of thumb” that can be used or sometimes recommendations from manufacturers. However, how those are calculated and what they are shooting at changes how useful they are in the real world. e.g. are you going to go for the most rigid machine you can find with perfect everything and the feed and speed numbers right before the tool breaks? That will give you a very impressive number… But realistically no one will ever be to use it. Do you instead go with the most conservate number trying to account for every possible penalty and give a number everyone could use? Well, that will leave a lot on the table, eat the tools, and give less than a desirable cuts for most of your users.
So how to get usable numbers… If we are talking about wood and kind of a random assortment of cutters we can use some basic rules of thumb and scale from there. The first thing would be what is our minimum chipload? Generally speaking the softer and more flexible the material the larger this has to be. Made better or worse by some of those “other factors” (see below). For domestic hardwood with decent tooling at least 0.1250" in diameter I’d say you are usually pretty safe starting out with a 0.002" (0.051mm) chipload. You can scale this as you go but other than a straight up metal cutter this will probably be at least cutting a chip with most tools. For RPM we have a huge range depending on the tool. For most decent tools we should be good to at least 800 SFM. This can scale up a LOT based on the tooling. But this will give us a starting point that should be safe. So let’s say that this is a 0.2500" 2 flute cutter. What that works out to is an RPM of ~12,000 and a feed of 48 IPM / 1219mm/m (RPM = (3.82 * SFM) / Diameter) (Feed = RPM * Chipload * Flutes). The best way to scale up from here is to actually test in YOUR material and YOUR machine.
The best way to do that in my opinion is to start off with a low pass depth (1 diameter or less) and test by scaling your chipload (feed). You will hit a limit of either the material failing (e.g. tear out) or cutting forces (machine or tool deflecting (bending)). If you aren’t at the deflection failure point then you can scale your cutting depth. Once you get this number back off at least 10% to allow for the extra cutting forces that will result from tool wear over time. This is what almost all production shops do but they will lock down a material supplier and tool manufacturer to reduce those variables.
Now I want to discuss some of those “other factors” that have to be considered. This is also why there is limited value in my opinion on thing like feed and speed charts or calculators other than maybe getting a baseline number (if they aren’t targeting a machine WAY outside of what you are using).
The first one is runout. This is how much the tool is spinning of the central axis of the spindle. Or how much the tool is wobbling. The reason that this matters is that in multi-flute tools this changes your chipload. It more or less adds and subtracts from different flutes chiploads at different point in the cut. Let’s use this in an example. Let’s say that we have a 2 flute cutter that we are going to run at 10,000 RPM and a 0.002" (0.051mm) chipload. That comes out to a feed of 40 IPM (1016mm/m). Now let’s say we have a total of 0.001" runout. That will make us cut a 0.001" (0.025mm) chipload on one flute and 0.003" (0.076mm) chipload on another (for at least part of the cut). That means that we will be simultaneously cutting at 20IPM (508mm/m) and 60IPM (1524mm/m) with our programed 40IPM (1016mm/m) cut. In some cases this will be okay and there’s enough room to absorb these changes. But it needs to be considered or you can end up with some really weird unexplainable results (cutting both too fast and too slow at the same time).
Material itself is also one of those other factors. It’s vastly more complicated than “hard” and “soft” wood. What really matters isn’t just the hardness of the wood but the component that the tree integrates into the wood, how well the wood stays together, the moisture content, grain tightness, etc. These will all change how the wood cuts. Again though, there’s some big margins in wood. So as long as you aren’t on the edge of something or trying to hit the peak of optimization it’s probably not going to be the biggest factor. However, it would be a good idea to look up things like the Janka value and try to keep an eye on the moisture content so that you can compensate you apply similar known working values to similar material.
Tool geometry is another issue. And honestly a very frustrating one from a user standpoint. There are TONS of variables that you are never going to see listed that effect things like the minimum chipload or max surface speed. These are things like rake, edge radius, helix, flute relief, core, etc. There’s also big differences in carbide grades even inside the same ISO grade. These all fundamentally change how a tool cuts. e.g. a tool with a lower edge radius and higher rake will cut soft material with a lower minimum chipload and produce less force for the same chipload. However, the skinner you get with this the more fragile the tool gets and the more likely that it doesn’t last in cutting say metal. There are some of these that you can check for with your own eyes. Things like helix (flute twist) are pretty easy to tell. And the tighter the helix gets the more force it is applying up or down. One of the big factors here is geometry that changes tool rigidity. The simple version of that is the more material remove the weaker the tool. So the tighter the helix, the deeper the cutting depth, and the deeper the flutes, the weaker the tool.
One of the other ones that’s often overlooked is your hold down method. Again if you are within margins you are fine. However, consider this with chipload. Anything that allows the material to “flex” or move a significant percent of your chipload can vary your chipload by that amount. As such I’m not a big fan of things like double sided tape as they tend to allow more flex than I’m comfortable with.
I’m going to end this here as this is already a massive text wall and I’m out of time at the moment. There’s more things and I can go into specifics if there’s desire for it. Let me know if there’s something you want expanded on or I can help with.
