There’s not enough info here for me to say definitively why. However, part of this may come from how little actual power is available from a router. Let’s use the Makita RT0701C as an example. It is listed as having “Maximum Horsepower of 1.25” (745.7 watts). However, this is typically measured as a peak draw for a very short amount of time. If we look at the actual input specs it’s 6.5 AMPS at we will assume 120V. That works out to 780w. However this is a brushed universal motor so let’s be forgiving and after all the losses we might have 60% of that left (~470w) to actually use at varying torque and RPM. If we take this with say 1/4" “generic” geometry tooling and try for an “optimal” cutting depth and chipload you could exceed this causing premature failure.
Don’t know what you were using or in what materials but I’ll try to give some insight on this. For the purpose of this I’m only going to touch on 3 things here and only the bare basics. Minimum chipload, cut quality, and tool wear.
Minimum chipload:
What I mean by minimum chipload is the least material were we can actually get the material to "cut" and not either grind or rub it out of the way. This is first determined by what is called the edge radius which is the leading edge of the flute. This is the first part of a minimum chipload as you can't cut a chip in any material thinner than the edge radius of the tool as you can't get "under" the material.
How small the edge radius is depends on the flute rake (angle of attack), grinding wheels used, carbide grade, and flute relief (material removes to keep the back of the flute from rubbing during the cut). So to make this more English understandable, we can’t grind the edge of the flute smaller than the grade of the carbide will support. Nor can we grind into that carbide finer features than the grinding wheel used. How those grinding wheels themselves are shaped to grind the carbide will also effect it and how many tools you can make before the wheels need to be reground or replaced. There are other things here too but this is already getting long winded.
The edge radius and the material properties will then determine the minimum chipload to actually “cut” a chip. The “softer” and more “flexible” the material the larger the chipload needed for the chip to support itself and cut. Additionally, the larger the edge and the lower the rake of the flute the larger the chip will need to be.
Cut quality
From a tool geometry perspective this will vary by many things but I'll go over a few common ones like the rake (angle of attack), helix (flute twist), flute relief (room made for the flute movement in cut), tool deflection (based on core remaining, flute volume, and carbide grade.).
A simple way of thinking of rake is how aggressive the cutting flute is. It comes at the cost of the strength of the flute. This will also along with the relief and edge radius effect the amount of force generated by the cut and therefore how much force the machine, tool, and material experience.
Helix is the twist rate of the flute. It’s effect on cut quality depends on the material, direction of the helix (up-cut, down-cut), and the relative strength of the CNC in Z vs X/Y. The tighter the helix the more shearing force and the more the force direction changes to the Z. The shearing force is almost always a good thing but the force direction can greatly change how a cut comes out. Too much for the material and you will start to tear-out, if the CNC is weaker in the Z than the X/Y then you may exceed the forces that the Z can resist without cutting errors.
The deflection is effected by the amount of material left in the tool (core), flute volume due to core and if you have enough room for the cut chips until evacuation, and the grade of the carbide as you pickup and lose features based on the cobalt percentages, carbide types and amounts, consistency and distribution of the powders before sintering, and the other added materials. Basically you have a base tool rigidity that is based on the carbide grade and then geometry effects that reduce it.
All of these will effect the cut quality in different ways and where the best quality and/or optimal cut is.
Tool wear
The carbide grade will effect this in a number of ways. First there's the hardness of the carbide that will effect the abrasion resistance to wear you will typically see this as a Rockwell A. Then there is the for lack of a better way to say it impact resistance. This is often not given but some manufacturers will list the facture toughness which is a decent analog. Then there's the carbide's ability to resist force before snapping usually listed as transverse rupture strength. This gives us a base to work with that the geometry then effects. As an example, if you have a very fine edge with a high rake that tool will loose it's edge faster. But some or all of that can be compensated for by picking a carbide grade with a higher hardness and impact or TRS depending on the tool application.
To give you a rough idea here’s the listed specs of a number of sub-micro grain carbides that are in the K20 ISO spec:
Chinese YG7
T.R.S= 1.9GPa HRA=90
Kennametal KFS06
T.R.S.=3.44GPa HRA=93.3
Ryotec (Mitsubishi) TF15
T.R.S.=4.0GPa HRA=91.0
These are clearly not the same and they will have a real effect on tool life. But how will depend on what they are used on and how they are used both from a tool geometry and chipload/surface speed standpoint.
All of the above being said it’s possible to have very different tool geometries and carbide grades and not make use of the differences thus leading to similar outcomes. As an example in deflection or power limited applications it’s harder to make use of even 1/4" tooling. You can’t really take deep passes and efficient chiploads leading to a lot of things averaging out if you try. However, if you change your pass depths and potentially stepover to reduce the forces you can still make use of the better chiploads which will result in better quality cuts and longer tool life. On the other end if you aren’t even getting to the minimums you will still remove material but you are basically using the end-mill as sand paper. You will never get good tool life that way nor be able to take advantage of any of the features of the geometry or carbide a tool might have. To be clear I’m not accusing you of this. I don’t have enough information to even have an idea if it would be true in your experience.
In this thread where we are dealing with features that effect the minimums. Losing some rake or increasing the edge radius here is much more critical as it effects the base chipload needed to make a cut that is multiplied by the chip thinning. So a cheap version of a tool might mean 50+ IPM difference between actually cutting or grinding.
This depends on the coating, the base carbide, and the wear method. I’ll give an example. Let’s say that we have a tool made for cutting domestic hardwoods and it has all the best possible features needed for this and is made out of a very good high hardness carbide. In most cases in that material we are not going to see any great increase in tool life for most coatings. This is due to the fact that we are both increasing the edge radius by coating the tool (you coat ALL of the tool), and that the wearing method is going to be more impact based than abrasive wear. So basically in that application we made the tool very slightly dull for no trade off. If instead we were cutting an exotic hardwood like say rosewood or ebony where the tree integrates silica into the wood, we would pickup more tool life as we are now in an abrasive material. This assumes though that we have a coating that is harder than the carbide, flexible enough to stay bound to the tool in the application, and can withstand the heat load. A lot of coatings do not have all those features. Some of them are specifically for metal where they rely on the heat generation to form an oxide that protects the tool. Some are so brittle that they can’t be used in applications where the impacts or flex in the carbide is enough to crack or otherwise compromise the coating. Some are also so temperature sensitive that they basically evaporate from the edge in some applications.
To be clear I’m not attacking your post. I actually understand where you are coming from. But there are actual differences for application specific tooling and premium tooling. Is it a match for your work, process, machine, material, and budget? I have no idea as I don’t know any of that in relation to you. But I hope the above will maybe help some to understand it better.
good luck hobby machines just that and I asked the 1f about a tolerance issue of circles and squares being .050 out of round and square and wanted to know how to fix it and they said to me via email it’s adequate for a hobby machines and wouldn’t offer any info to fix it sad but true I thought these machines were more accurate than .050 I can hold closer tolerances with my skill saw 
