A few corrections in turn (this is why peer review of board design is aways a good idea!) There is a trace missing, and the CPU power connections short reset to VCC (off by one pin) and produce ground loops (where one pin has 2 or more parallel connections to another pin.) This is your 0.28 version with the problems circled:
The “one net to route message” (circled in blue at the bottom of the window) is because of the missing trace between R1 and the ON LED. The red/blue circled trace on the CPU is off by one, and shorts Reset to VCC. The two red circled traces cause a VCC ground loop where there are two different current paths to the same pin. This can be a problem (especially on power and ground) when high current causes a voltage drop across the traces. With two paths, current will flow in the higher resistance path to the lower voltage which is very undesirable. All connections should only have a single path to any other pin (no parallel connections.) Once those were corrected, I cleaned up the routing to meet best practices. Best practice is that connections to a pad should be at right angles, and intersections in traces should be at 45 degrees (which is really most important at rf frequencies, but always doing it is the best practice, plus it reduces EMI if that is important to you.) or at 90 degrees for a straight run. Since this is a reference design it is desirable that it meet best practices to serve as an example. In addition I increased the trace size of all the power pins in to the CPU from 8mil to 12mil (the same size as the trace to the pins.) That provides a bit more current carrying capacity at no particular cost. It may be an idea to create a ground fill on the top of the board. That would increase (greatly!) the copper available to heat sink the regulators with the only cost being the hassle of adding the ground fill.
This snippet indicates the correct way (the top and bottom pads outlined in blue) and the wrong way, (the middle pad entering at 45 degrees.) Because of the fine grid size (0.25mm) insuring that the traces are straight is a challenge. The ruler in core parts provides a convenient way to achieve straightness (at least as much as we can!):
here the top layer trace circled in red is a little high on one side.
clicking and dragging it a bit straightens it up to exactly horizontal. Here is a version 0.29 of the board with these changes made (and hopefully no errors added .)
ARDUINO-MEGA-MINIMALISTE-Fritzing-V0.29.fzz (128.7 KB)
One final suggestion, what may make a good reference design is to add 1.27mm pitch (0.05in, half the size of standard .1in headers) for all the I/O pins to make a complete ATmega mini board with the I/O pins out to headers just like a full size ATmega. The down side to the 1.27mm headers is that there are no (that I know of) patch cables for them. I made some (because I have wireless modules with 1.27mm connectors) out of a bunch of single pin milmax single pin solder connectors (with the other end being a standard .1 header connector) but they are $2 Canadian each (when I bought 25 the first time they were $1 ea at mouser, but they now match digikey at $2 ea!) This is the only single pin 1.27mm jack I know of though.