How do I ensure the schematics and PCB in my project are synchronized?

Problem:
After importing a PCB project from another vendor (such as OrCAD or P-CAD), or during routine Altium Designer PCB project editing, it is often desirable to check the status of the differences between the schematic set and PCB. What is the easiest way to do this?

Solution:
This process is often referred to as design synchronization.

Synchronizing a design requires two steps.
1) Make sure all schematic components and PCB footprints are linked using Project > component links and
2) Using Project > show differences to resolve any other differences, based on the project options.

Here is an example case that describes the synchronization process after importing a P-CAD PCB project which contained three schematics and one PCB.

Import the P-CAD files (one .sch and one .pcb file) using the Altium Designer Import Wizard (File >> Import Wizard). It created an AD PCB project. I examined the project and decided to discard the (unnecessary) top level schematic sheet that had been created during the translation process. The top level schematic sheet just had three sheet symbols on it. It is created in case you want to use a hierarchical schematic sheet structure rather than a flat design. Since there are only three schematic sheets, a flat design strucure is fine. More than six schematic sheets and I like to go hierarchical.
I synchronized the design by first ensuring that the unique identifiers on the schematic match those on the PCB. In Altium Designer, each schematic symbol and its matching PCB footprint share a common unique identifer. They're necessary in case you change the reference designator. P-CAD doesn't use these.
You do this by first opening the PCB, and going to the menu bar, Project >> Component links. This brings up a dialog box where you will be able to map all unmatched components. The goal is get all components in the 'Matched Components' column on the far right. If your P-CAD schematics and PCB had all matching designators, you just have to click the button that says 'Add Matched pairs By >>' and check the designator box, then click 'Perform Update'. All components will switch from the unmatched column to the matched column on the right.
Step 2 to synchronize is simply to ensure that there are 'No Differences' between the schematic and PCB, as follows.
In either a schematic or the PCB, go to the menu bar, Project >> Show differences. This launches a small pop-up called 'Choose Documents to Compare', where you choose the PCB in your project and click OK. This will launch the Differences dialog box where you examine the differences between the info in your schematic set vs. your PCB. There may be quite a few, but many of them will not be a real problem because they describe differences that do not effect the electrical connectivity of the design.

At that point, I just went to Project > Project Options, comparator tab and set some of the project settings to ignore the differences between things like different comments on the schematic component and the PCB footprint.
The goal is to be able to run Project > Show differences and see the pop-up 'No differences detected'. If there are differences, just make sure you know what they are and they will not adversely effect the integrity of your design.

For example, if show differences tells you that r1 has different comments, I don't care. It doesn't matter if the r1 schematic component comment says 100 ohm and the r1 footprint comment says 0805. But if Show Differences says that the schematic component r1 exists in the schematic but not in the PCB, that's something that will command more attention.