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.
I’m not sure you know how deep this rabbit hole goes…
I’ll first try to address this without tool much techno-babble. That feed and speed works out to a 0.0025" chipload. That is extremely conservative for a 1/4" tool in wood (depending on pass depth). However, the RPM is somewhat aggressive at 1178SFM. Might be fine depending on the tool geometry. If it were me, I’d at least double the chipload (feed) without an increase to the RPM. All of that though has to be balanced against the pass depth to control cutting forces. You don’t have one listed here. So I’m not sure what you need to hit or really have a decent point for advise.
Also, as djdelorie pointed out you have a lot of margin here. Even the 0.0025" chipload is above the “minimum” for rubbing, depending on artwork (direction changes and acceleration).
Techno-babble…
What you have in your last post is chipload formulas. This along with surface speed is what all feed/speed are trying to get to. Probably in almost all cases chipload is the MOST important factor in milling. So yes you could use that formula for an increase in RPM keeping the same chipload.
The answer to your general question though isn’t as simple as that. The short version is that every material and tool geometry will have a “sweet spot” where it will cut well. There are MANY variables and no completely easy rules of thumb. As an example let’s say that that 90IPM at 18KRPM is is good number (although it’s a really low chipload). If you changed one aspect of that tool like it’s rake (flute angle of attack) or helix (flute twist) that number will no longer be correct. Or at the very least it would change where you get the most productive or best finish cut.
As mentioned you have a decent amount of margin in chipload in this size in soft media. However, you need to keep a minimum chipload to prevent rubbing. Basically if you don’t cut a large enough chipload you won’t actually be cutting a chip. Instead you will rub the material out of the way functionally turning your endmill into glorified sandpaper.
The RPM question comes down to surface speed. Surface speed is the speed of the edge of the cutter. So for the same RPM, the bigger the tool the higher the surface speed. There are pros and cons to higher surface speed depending on the material and cutter. The short simplified version is that geometry changes like rake or edge radius along with the material determine where you can run it without damaging the tool or material regardless of chipload (feed). Again, an extremely simplified version would be that the more “aggressive” the tool, the higher your surface speed can get. Most of those though come with weakening the flute or tool. There’s also an increase in sear force with surface speed. In soft materials that can help get a clean cut.
What the combination of those comes to is that you want as high a surface speed as you can get, while still supporting a good chipload, and not exceeding the tool design or material strength.
Ignoring the surface speed for a moment. The rest of this comes down to exceeding the minimum to actually “cut” a chip while keeping cutting forces in check for the tool and machine. More or less this comes down to cubic material removed per flute per rotation. So we have an increase in cutting forces for any increase in chipload, stepover, or pass depth. Those forces have to be resisted by the tool and machine. When they get out of control they start to effect the cut with things like chatter. Bigger chiploads though will usually leave a better cut, cut faster, and increase tool life. At least up until you reach a limit for the material, machine or tool.
There’s also a bunch of other variables like runout which can add and subtract chipload from flutes in multi-flute cutters. Or tool geometry variables, carbide grade, coatings, tool tolerances, etc.
That all works out to if you REALLY want the “BEST” cut for YOUR material, on YOUR machine, with YOUR tool, you are going to be testing. Unless your in a production mode though, that might not be the best use of your time and resources.
I rambled enough. Hopefully some part of that was useful to someone. If there’s something I can expand on or help with let me know.
