Close, but not the exact problem.
When I first open the schematic, it looks like:
When I view the properties of one of the [ ?? ] symbols, I see it references the Emetcon library, which is present in the project.
Eeschema / Preferences / Manage Symbol Libraries / Project Specific Libraries / "Add existing Library (icon) fixes it.
The links for project specific libraries are saved in the “sym-lib-table” file inside your project. Do not delete that file.
Even better: Never delete files of which you do not know the purpose.
Your schematic passes ERC without problems. That is good.
I always try to have high voltages in the top, and lower voltages in the bottom, and have signal flow from left to right. That does not work for the microprocessor, but it can work for the power supply.
For example, you have the power connector in the rightmost corner of the schematic and your decoupling capacitors rotated (and in two rows). The way you did it is not wrong, but keeping the top - down voltage flow and left - right signal flow makes the schematic easier to read and check, and thus the chance of errors smaller.
You have a bunch of long wires near your busses, with Reset, R/W, CLK, and some other signals. These are hard to follow. Working more with labels here is a good idea.
Connecting the 1MHz clock to the enable signals of the memory IC’s? Looks weird, but I am not very familiar anymore with these old IC’s.
Why use optocoupler U9 if you connect the “other” side to GND anyway?
No RAM IC? Does the HC11 have internal ram?
What is this thing supposed to do? Your MCHC11F1 has over 30 unused pins. Are these generic I/O? Maybe put connectors on these so it’s easier to use them for “something”. On the PCB it looks like a PLCC socket and the SMT parts are hard to reach.
Your PCB passes DRC with no errors, that is always a good thing.
Your power connector J1 is a regular 0.1" header. Use a better power connector here.
Your PCB is quite big with lots of space in between the parts. There is nothing wrong with this in itself. For the most part, the PCB will be a bit more expensive, but it’s also much easier to design and to route the tracks.
As Eelik already mentioned, the absence of a GND plane is quite bad. Adding a decent GND plane is the single most upgrade for this design. There is lots of documentation about GND planes and signal integrity. It is not an easy subject to grasp, but it is very important.