If your Drawing is showing dotted line boxes with an X through them, or if your Assembly opens with some components suppressed, then it's lost it's reference to that file (or files). It was probably either moved or re-named. If it's a Drawing, close the file, then go to File > Open. Browse to the Drawing and select it, but don't open it. A "References" button will appear near the bottom of the Browse window.
Click on it. That will open another dialog box with all dependent files listed in one column and their location in another one. If the file was re-named you can double-click on the file name in this table and select the new name from the Browse dialog box. If it was moved double-click on the appropriate cell in the "In Folder" column instead, and Browse to the correct location.
For Assemblies there's another method you might prefer, but it only works if the file was moved, not if it was re-named. Try un-suppressing the component. You might or might not get a message asking if you want to find the component. If you do, of course do so. If you don't, go ahead and browse to the component and open it. Now go back to the Assembly and un-suppress it. If there's more than one instance of this component you'll need to un-suppress each one. If this doesn't work for some reason, use the same method described above for Drawings.
In the future if you want to move or re-name a file do so by right-clicking on the file in Windows Explorer, going to Solidworks in the drop-down, and selecting the appropriate option in the fly-out menu. Another method for re-naming components in Assemblies is to do so directly in the Assembly tree. You will need to make sure you have the option selected allowing you to do so at Tools > Options > System Options > FeatureManager.
Then make sure the option below is also turned on (I can't imagine why there's an option to not have them update).