I copied my work from my school computer to my home computer. Because of that my drawing files don't know where to find the part files. I used to get a pop up window that asks me to browse for the part file, but I clicked the don't show this again option. I don't know where to find that again.
You can hit this button in your drawing and browse for your part file
It still doesn't put all the views in the proper place.
Issue #1: Part and Drawing files. The drawing file is looking for the part file. It knows the name of the part file and it is looking for it in a particular location, but it is not there. Instead of opening the drawing file on your home computer FIRST open the part file, then open the drawing file. The drawing file will see the part file that is active and open in SWX and will therefore not need to look for it (and it would have been looking for it in the wrong place anyway). If your part and drawing files are stored in the same directory at school and they are stored in the same directory at home then when you open the drawing file it should automatically find the part file, even if the school and home directories are named differently. Apparently the problem you are having is because the part and drawing files are not stored in the same directory at school or they are not stored in the same directory at home.
Issue #2:
I tried opening the part first. I also went into the settings you showed me, but it still won't show that pop up again.
When you open your drawing, look for the "References..." button and select it and you can pick your part or parts to load.
Eric, this is the "old school" way of doing things, I still use it, and it works every time! Thanks Tony Cantrell
You said "I copied my work from my school computer to my home computer." What method did you use for copying, and did you copy all the models along with the drawing? Next time I'd advise using Pack and Go to keep the relations.
Eric, Glenn asked the right question because the several methods described to you should have easily worked. Do you have BOTH the part and the drawing files? How DID you copy them? Could you have multiple versions on your school computer and possibly grabbed disconnected versions?
Uploaded to google drive then downloaded from google drive.
Eric, I'll ask you again. Do you have BOTH the part and the drawing files? How DID you copy them? (Answered: Google Drive) Could you have multiple versions on your school computer and possibly grabbed disconnected versions?
I assume you are still having the issue because you have not indicated otherwise. About the only way the part and drawings can be disconnected is if they are not stored in the same directory arrangement, or if the drawing is looking for a part file named differently than what you have.
HOWEVER, the directions already given you will fix either of these situations if you follow them properly.
Dare I suggest you post both files and let us connect them?
I'm pretty sure I only have one file for each. Could it have come disconnected when I reorganized my files and folders?
I'll post both files. Either connect them and tell me how you did it or lead me to the answer or just whatever will help me learn most.
My prediction: It will open up a window. You select browse for file. It connects just fine. Mine still won't connect.
Eric,
In the tree on your drawing RMB and choose show.
Since it asked me if I was sure I wanted to save I am assuming I am on a future version of software. Your views are hidden for some reason.
When you renamed the folders or files, SOLIDWORKS "lost the connection" - use the techniques above to "re-connect", as soon as you save, everything will be right again.
todd
Steps I followed:
1. Put both unzipped files in the same directory.
2. Opened the Knob part file.
3. Tried to open its drawing file but it did not know there was one. (This tells me they must have been in different directories at your school.)
4. Opened the drawing file and saw this:
5. In the drawing file went to the top to File -> Find References and saw this:
This tells me the drawing is indeed looking for a part file named knob. It does not explain why the views aren't showing.
6. RMB on each drawing view and selected Show and got this:
I don't know how all your views got set to hidden, but they were, at least for me.
Now, you still have not fixed the clocking of the keyway (the sketch is under constrained, but you'll have to edit the Library Feature and uncheck this box in order to fix it).
You'll want to fix these:
You haven't yet addressed a lot of the other things that have been pointed out about this drawing in your other posts, including moving extension lines off the object lines:
That is enough from me for now.
Eric,
Glad I could help.Perusing some of your other posts you have asked for help on drawings(prints) for parts. 
I changed your back view on mine with the changes shown. Decimal place aside, a hole is a hole not a radius. Dimensional tolerance gets doubled for a hole if it is called out at a radius. Plus you do not want people taking a calculator to figure out sizing if not necessary. Machinery's handbook has all of the information on keys you could ever want. You have to clock your key so you need a way of showing that on your print. Also on your overall print there is no relationship established where this view even comes from. These are just some pointers. Good luck.
p.s. In your title block: two place decimal +/-.05 three place decimal +/-.005. (This is why I said decimal place aside above) Everything on your drawing is 2 place or looser. Very rare on a hole with a key.
Eric,
In the tree on your drawing RMB and choose show.
Since it asked me if I was sure I wanted to save I am assuming I am on a future version of software. Your views are hidden for some reason.