Well. the fact is that in computer compensation allows you to specifically construct tool path to avoid gouges and crashes in confined spaces so you have more control and outcome is decided before tool touches stock.
As you noted, making a strait cut to see that tool is on proper diameter is something I do daily, I can measure that and I can measure depth from face, from there any arc and taper is going to be accurate providing tool radius is not deformed or chipped, has uniform amount of stock across entire path and type of material doesn't wear out tip before tool reaches end of the cut.
You can achieve same thing by use of in control compensation with potential setbacks.
One area where you seem to have miss conception is wear offset as related to radius of insert.
For instance, using end mill and programming its center point, then using diameter or radius in machine control is not the same as using radius tip on lathe.
When end mill wears out by .001, you can measure it and correct for it in wear offset or by adjusting diameter or radius value.
You cannot measure insert radius while it is mounted in tool, therefore you don't know by how much to adjust wear offset or radius value.
In 99% of lathe work I program "imaginary tool nose", the point where two lines intersect each other at 90 degree as insert touches each line, one representing X axis and one representing Z axis.
This is in sink with how tools are touched off on probe or by cut and measure method.
On rare occasion, I program tip or center point of round insert, for reasons like associating print dimension with tool position and strait plunge.
Now, on mill you are compensating for tool radius, on lathe you are compensating for difference between that imaginary programmed point and all points along insert tip radius.
Every possible taper angle between 0 and 90 degree has different compensation value for given size of insert radius and it is calculated in computer (or at the machine if you use in control compensation).
You can find these values in increment of one degree in the back of the Bible (Machinery's handbook), for example, 45 degree compensation for 1/64" radius is .0092, if I am cutting .1 chamfer on outside edge and using direct compensation, chamfer value in Z axis is .1092, and .2184 X axis, diameter programming.
Same chamfer is programmed as .1 in Z value and .2 in X value with .0156 entered in radius field of machine offset page and tool being used along with correct tip number for orientation, tip # 3 in case of turning tool.
I started in days of DOS and trigonometry on scratch paper by the machine, so I am fully capable of programming a job using "in my head" compensation we now call "in computer", the difference is that I am now more efficient and more accurate.
That was all in relation to tapers, for any arcs I use IJK since beginning, IJK values are signed incremental distances from center of the arc being cut to center of the tool radius when tool is at start point of an arc.
You subtract tool radius from programmed arc move for concave arc and you add it to arc value for convex arc, that simple.
There is a miss conception of "easier method" being attributed to in control compensation, in part because you don't have to calculate it and in part because you can program dimensions strait from print.
This leaves it for machine and on the fly calculations to figure out what you did not and when there is a problem, you have a gouge on part or interrupted finish pass which you have to recover, fix the problem and repeat without showing tool mark or loosing size.
As I sad, you can accomplish same result using either method as they are essentially the same concept, the difference is in being in control ahead of the game or reacting to event you cannot always recover from without damage.
One commonly observed problem with in control compensation is that in cutting partial arcs, machine tends to dive as deep or as high as it wants with no regard to surrounding features and clearances.
Small shift in direction of cut can easily results in goudge and both are easy to overlook while dry running program and before it is too late.
For years, I used computers with progressively more sophisticated software, in early 1990 I even produced peace of software compiled in Microsoft Basic that helped me calculate tool paths for C axis work, actual G code produced based on tool diameter, stock diameter and measurements across flats of hexagon, square or two flats, done in polar mode as very common features on mill-turn,..... even had cutter compensation included in G code.
I had HP LX-95 handheld computer running DOS 3, screen size was 2" x 4" if I recall correctly and I dished out close to $500 for it, it was "must have" gadget for any wannabe computer geek.
So, I'll take computers any day, over old, in control compensation method, to me that's working harder and I don't like to work harder then I have to and come up with same result or even fall short.
Why not take advantage of detailed graphics, controlled tool paths, simulation, backplotting?, polish every move with accuracy and visual confirmation before tool makes a single chip.
Any argument you can think of in favor of in control compensation method flies right by me as it has no merit in my book at this day and age but that should not stop you from believing in it ...... and working harder.
