The category here is “parts submit”, but seems like a good place for something like this as well. The paragraph is just the post content that goes with the uploaded file. It needs to be outside of the sketch itself, so searches (in the forum, or from google) can find it.
According to the wiring on the other views, you are missing a trace on pcb view. Fritzing tells you about that with the status information at the bottom (“26 of 27 nets routed - 1 connection still to be routed”). It is the top 2 ground connections in the 2nd column from the right.
One of the general rules / conventions / goals for pcb traces, is to avoid 90 degree corners where possible. Shallow angles are preferred.
Looking closely in all of the views, you have some extra bend points in wires right on top of connection terminals, or bend points on top of bend points. Those can be seen by moving the part, and seeing that the wire leaves a bend point behind at the connection point.
You have used single row, single pin headers for a lot of the connections. Using a single row, multiple pin part would simplify positioning, and make sure the the proper spacing is maintained. Although that would make the schematic and breadboard wire more complex / messy, tt would simplify the “BOM” for the pcb board.
The text note on the PCB view has some spelling mistakes. Here is what I think it should say.
This is a breakout PCB for MCP23017 made with a DIP instead of an SMB. All important pins are on one line so it is stackable on a mainboard. For using multiple breakout boards together A0,A1,A2 are reorganised for easy configuration with jumper pins.
DIL is “dual inline”, DIP is “dual inline package”.
For me, since (at least) Canadian and British English spell “reorganised” as “reorganized”, there should be one more change.
For some reason, your parts are not quite aligned to the main 0.1 in (or 2.54mm) grid. If that was done to assist in getting the traces to “centre” between rows of pins, that is the reason I said I set the grid spacing to half of what I really wanted to use. You set grid spacing (at the end at least) to 0.508mm, which is 0.01in. For something like this, I would have used fractional inch units, just to keep the numbers simpler.
I played with your sketch. Here is my version using your layout and routing, but with a few tweaks to positioning and labels. I adjusted the grid size to different values when working on different sections. 0.1, 0.025, 0.02, 0.021 inch. Since some of the headers are now longer, I replaced the associated part labels with separate silkscreen text parts. That needed adjustments to the other views as well.
MCP23017-BreakOut-Vertical-Stackable-V2.fzz (47.1 KB)
I don’t know if you are trying for an exact match to an existing board, but I would have used 3 headers of 3 pins each for the address configuration. Ground at one end, an address line in the middle, and Vcc at the other end of each header. With a 0.05 or 0.1 inch separation between the headers. Those do not need to stay on the same grid as the stackable headers.