There are plenty options here.
- Start with a template, that has outline, mounting holes critical connector locations, and use that template for both projects (probably a bit late now).
- Generate gerbers from both projects, and then load some layers from those projects in the gerber viewer and lay them on top of each other.
- The Gerber viewer can create a PCB from a set of gerber files, but that does not give more possibilities in this regard then doing something with the original files in the first place.
- When the PCB editor is running in Standalone Mode you can use the File / Append Board function to load another PCB. (Make sure you have copies, backups).
- You can use: PCB Editor / File / Fabrication Outputs / Gerber / Plot Format: SVG, and then in the other project, use PCB Editor / File / Import / Graphics to read your image and put it on a user layer for reference.
These methods can all be used to verify whether things were done correctly, but for designing the thing in the first place, putting both PCB’s in the same location on the canvas makes it easy to directly compare coordinates. Using the “File / Drill origin” and put it on a reference location (for example pin one of the mating connectors) is also a good option. And there are some left over risks that have to be managed. For example when using dual row pin headers, you can either put both connectors on the top of the PCB of each project (such as those “stack through” connectors used in PC104), or put one of the connectors on the bottom, but you have to use Male / Female connectors to prevent mirroring the pin layout.
Doing a manual test with something physical you can touch can also help, such as:
Also, mating the connectors before and during soldering can help. It reduces the risk of the plastic overheating, because the mating connector absorbs some of the heat. And even if they overheat and some plastic melts, it still keeps the conductors in the right place. It also improves alignment during soldering.