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.
This is a remarkably hard question to give a simple answer to. The problem is that you have a huge number of variables that can change what you should actually be running at. I’ll briefly go into some and link to other posts I’ve made to keep this one from being too long.
The thing I would say is the most important to understand digging into feed and speeds is chipload. The simple version is that chipload is the thickest part of the chip removed from the material per flute per rotation. This combined with surface speed is ultimately what all feed and speeds are trying to get to. As an example if you have a feed and speed of 100IPM (2540mm/m) at 20KRPM for a 2 flute in a given material that is a 0.0025" (0.0635mm) chipload (Feed / RPM / Flutes). That chipload number will mean more to the cut than anything else and can be scaled with RPM up and down for the machine and surface speed.
What chipload will be good for a given material will depend on not just the material but the tool geometry. A few simple examples of this would be rake and helix. The rake of the tool is how aggressive the cutting flute is. The higher it is the lower the forces to cut a material. It comes at the cost of flute strength though. The helix is the twist of the flutes. The more there is the higher the shear forces and force direction changes. This can help to drive more of the forces into the Z and cut material cleaner. However, it comes at the cost of tool strength and if the helix is too high for your material you will start to tear out since more of the forces are moved to the Z. To summarize those examples in their own example. Let’s say we are cutting wood. It will cut better and with less forces using a higher rake tool. You also want at least some helix as that will increase your shear and spread the load to the Z. However, you want to avoid high helix tools as the material won’t be able to hold itself together with too much force in the Z.
After that you have material considerations. Woods are notoriously more problematic as they aren’t consistent. For simple examples again you have hardness (janka), the grain (tightness and direction), and moisture content. Every one of those will change the correct chipload for the material. The hardness is a fairly obvious issue but I don’t think most people realize the true range. Pines are around 350-700lbf, maples 700-1500lbf, oak 1000-1500lbf, hickory 1300-2000lbf, and rosewood 2200-2800. That’s not the top and bottom and I’m chopping part of the ranges. Then you have the grain which will cut differently and have parts that are hard and softer so how “tight” the gain is effect how you can actually cut it (e.g. maple generally cuts cleaner than oak even with the same hardness). The moisture content also changes the cutting dynamics with dryer wood preferred for consistency and tool life. Plastics and metals are more consistent but both still have minimum chiploads you need to hit to keep from melting and to actually cut and not grind.
You then have machine and tool force limits. Assuming there’s not a material limit you are then going to run up against cutting forces. First the tool obviously has a limit before the force on the flute breaks it. You also have a tool deflection which is how much the carbide is bending from the forces of the cut. The tool deflection is also effect by geometry and carbide grade. Those forces also have to be resisted by the machine and it will also deflect (all machines do). How much deflection you can get away with will depend on your tolerances and finish requirements. Eventually it will be enough to cause chatter and/or enough deflection will break the tool as it snaps back to it’s normal position as it slows during cuts.
After all that you have modifiers like runout (how much the tool is spinning of the center axis of rotation). Which can functionally add and subtract an unintended chipload (feed) in multi flute cutters.
All that to basically say there’s not really any great calculators out there as they are pretty much all missing data that changes where your good/best cut will be in YOUR material, with YOUR CNC, and YOUR tooling. So in general it’s better to try and find a decent minimum and work from there.
To answer some specific questions here:
No, you will regularly see industrial machines run well over double or triple that at 0.50" pass depths with good 1/4" tooling. Can you? That depends on a lot but you will reach a machine deflection limit before those machines.
Keep in mind chipload here 110IPM at 18KRPM on a 3 flute is a 0.002" (0.05mm) chipload. That’s barley the rule of thumb minimum for soft material and it won’t maintain it in direction changes. The 30IPM is obviously under it (I’m guessing 30 is a typo).
A IPM range without RPM and flute count means nothing as it’s ultimately chipload.
If a tool “screams” or not is usually related to surface speed, chipload, and geometry. So it will scream in general if you just have much too small of a chipload. However, it will also scream even at a good chipload if the RPM is too high for the geometry. There’s also cases in extremely high aspect ratio tools where you are just screwed noise level wise no matter what.
The short simple version would be that you can treat them proportionally. Until you reach the material limit this comes down to force. The force is mostly cubic material removed per flute per rotation. So if you chop the pass depth by half you can double the feed. It’s not exactly a 1:1 as the helix plays into it but it’s pretty close.
Here’s some of my posts I was talking about to keep from making this one longer.
More on chiploads and surface speeds. Origin/consistency of chipload recommendations - #285 by TDA
More on runout. Precision collet upgrade worthwhile? - #12 by TDA
Deeper break down of some tool geometry and material effects. Best practice for tiny endmills - #15 by TDA
I’ll end this the same way I did on chipload thread. Don’t get bogged down in the optimal or perfect. There are pretty big margins with decent tools in soft material. That not to say you can’t get some more knowledge and get a better result though.
Hope that’s useful. Let me know if there’s something I can help with or expand on.