If your Assembly shows some components suppressed and you can't un-suppress them, or if your Drawing is showing dotted line boxes instead of your drawing views, then it's lost the link to the dependent files. You or a coworker probably improperly moved or re-named the files, although there could be other reasons. However, assuming you know where the files went (or what they got re-named to), it's easy enough to restore the links. One method is to close the file and go to File > Open. Browse to the file and select it so it's highlighted, but don't open it. Click on the "References" button.
That will open another dialog box, with all dependent files listed, along with their folder locations.
If the file was renamed then double-click on the file name and select the new name from the Browse dialog box. If it was moved then double-click on the folder name string instead and Browse to the new location. If more than one reference was lost you'll need to do this for each one.
For Assemblies, there's another method that you might want to try. As I said above, if SW has lost the reference to components then they'll come in suppressed. You can try to click on them and choose the "Unsuppress" icon. Prior to SW2018 when doing this I'd get a message box asking if I wanted to find the component myself, so I could browse to and select it, and it worked fine. However, maybe it's just me, but starting with SW2018 I don't always get that message box. Nothing happens when I try to unsuppress. However, I've learned that I can open the Part, then go back to the Assembly, and I can unsuppress. If that component had been patterned then the pattern will likely show an error (see below). You can manually suppress the pattern and then unsuppress it, or expand it and unsuppress the components, and the error will go away.
In the future, if you want to move or rename files while maintaining the links do so in SolidWorks Explorer, or right-click on the file name in Windows Explorer and choose SolidWorks > Rename... (or Move...). However, this option will only be available if you have SolidWorks Explorer installed. Depending on your Search parameters this might also not find all references.
Beginning with SW2016, another alternative for Assemblies is renaming the dependent files directly in the Assembly (see here). I've had good luck with this option. I have fond hopes that at some point in the future we'll be able to use a similar workflow to rename files from a Drawing, but so far (as of SW2018) that's not available.