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.
There’s not really enough data here to give what I would consider a good response. (no number of flutes listed, no material given, no info on tool geometry). The flute counts are needed for chipload. Material is needed for minimum chiploads, wear effects, force estimates, etc. How hard you can actually push a tool in deflection or power limited application depends on things like rake, helix, carbide grade, etc. As an example a higher helix (flute twist) will start to tear out at a lower feed (yes even with compression tools). I’ll break down what I can and make assumptions for examples.
The above being said I’m going to assume that the 1/4" is a 2 flute cutter with a “generic” geometry. Making that assumption here’s what the chipload and MRR (material removal rate) looks like for the listed cuts (skipping the V cutter).
Whiteside 6210 - 0.0013" chipload - 2.14³in/m MRR
“Chinese” compression ADV V - 0.002" chipload - 0.90³in/m MRR
“Chinese” compression Profile - 0.002" chipload - 2.25³in/m MRR
The first obvious thing here would be that if you are not having an issue with the profile cut, get rid of the stepover in the V carve for the 1/4" tool. That over doubles the MRR which will let you finish that part of the cut faster.
In general, I would say these are all very conservative assuming soft material (wood, plastic, etc). Normally I would start most people out at double that chipload on a 1/4" tool (depending on material, CNC, etc). Most tooling should be able to easily handle that or more. There also shouldn’t be an issue with the machine or the router either. To give you an idea, in production cases with good tooling a 1/4" tool is capable of over a 0.012" chipload. What you can run at ultimately depends on the tooling, material, and where you hit a deflection (bending) limit.
Making the assumption that you can run the 0.004" chipload on the 1/4" it renders the surfacing bit useless. The MRR with the 1/4" tool, 18KRPM, 0.004" chipload (144IPM feed), 50% stepover, and 0.125" pass depth is 2.25³in/m which is greater than the surfacing bit. It also skips a tool change.
Another quick change to this would be to go to 3 flute tooling if you have enough feed available. At the same settings as the above that result in a MRR of 3.375³in/m with a feed of 216IPM. Could also scale this some with RPM to hit a lower feed.
Those are just starting numbers though based on what you already listed. If it were me I would test increasing the feed until I got a cut quality issue, then go and see how far I could plunge per pass with that feed.
You could also potentially save time and money switching cutters in other ways. But it’s hard to make any real comparisons or point out what features to look for without knowing the material, existing tooling, or issues.
One other thing. Depending on the material and tooling you are almost certainly running too high RPM for both those cutters. The surface speed on the 1" cutter is 4712 SFM and on the 1/4" it’s 1178 SFM. Might be okay on the 1/4" depending on the geometry and the material. This will eat tooling and potentially leave a bad quality cut. Can’t give you a specific number due to the missing data but a middle of the road one would be around 800 SFM (~3KRPM of the 1" and ~12KRPM for the 1/4"). This would be another good reason to get rid of the surfacing tool in this application.
Hope that’s useful. Let me know if there’s something I can help with.