I'm attaching here some templates for SolidWorkers who find themselves with only the default templates. These are mostly aimed at small-company users, with small printers, and with an informal drawing requirements structure. I minimized the junk to maximize the usable space.  e.g. Often many of the sign-off fields (Mfg Approval, QA Approval...)  for drawing checking are left blank. One cool thing is I made these templates in SolidWorks 2015, so more users will be able to open.

The two most essential files, from which all the others could be recreated:

A-sheet1-2015.drwdot   (8.5x11" paper)

Legal-sheet1.drwdot     (8.5x14" paper)

You have a functional ANSI drawing template with just one of these files. But it can be set up a little smoother if you make use of sheet formats (for example to change the paper size of an existing drawing, or to make sheet 2 layout different than sheet 1). And best if you have assembly and part templates with matching text "Custom Properties".

You can change any of the "dot" template filenames without consequence (.drwdot, .prtdot, .asmdot).

.slddrt format files may have a .drwdot that defaults to looking for their specific filename (but they aren't closely linked, the format isn't needed all the time, just occasionally it is helpful).

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Main things to change for your own use:

+ Change company name two places (legal ownership statement, and big in title block).

And ideally...  

+ Change the path to the sheet format. Do this in the .drwdot Sheet Properties  (select "Properties by right click in drawing, or right click on Sheet1 in tree).

I personally put sheet formats (.slddrt) and drawing templates (.drwdot) in the same folder for simplicity, and I usually give them the same file names.  The folders should be where you are pointing SolidWorks for System Options >> File Locations >> Document Templates, and System Options >> File Locations >> Sheet Formats. 

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Some sheet formats are included for examples, but you should edit the templates (File >> Open >> Drop Down select Template), and then use Save Sheet Format and create new ones. (And then edit the .drwdot sheet properties to look for your new format, and resave the .drwdot).   Sketch in more title block lines if you like. 

After your changes, you don't need to keep a .drwdot for sheet 2, but I kept it in case you want to mess around with it.   Removing it is mainly to simplify user choices when picking a template.

I left enough space in Revision field for a date without punctuation (YYYYMMDD).

10 digits in part number.

I like the expanding Material field for the rare detailed specification, you might not.  

Properties.txt is just for convenience, to populate the Custom Properties drop down.  Most are defaults that SolidWorks started with, I added a few. This goes in the folder indicated in System Options >> File Locations >> Custom Property FIles (rename the original as a backup first). 

There are a few Layers. With "Per Standard" active all dimensions will be added to the Dim layer (which is black). 

Watermark is a block because that pushes it to the back as far as visibility - so you can see dimensions on top of it.   It is set to use the Redline Layer, mainly to make it red.  Edit the text in the drawing file custom properties.

Most of the title block fields are file based text properties that are controlled by the model (.sldprt or .sldasm).

DrawnBy, DrawnDate, and Watermark are drawing based.

The drawing title block is live, so double click inside the orange border that pops up and you can edit text fields.

Things I did not do:

- Set up BOM tables and Revision tables... 

- I didn't use these extensively to find all the little things one could tweak (balloon size, fonts size, etc). 

- I only have inch versions ready, but metric is a pretty easy change - Other than drawing units, the tolerances need be adjusted.

- 11x17 (ANSI B) is a great size, but I don't currently have a printer that can do it.

- If you have a newer SolidWorks there are some great settings that you may want to change - like in ~2017 they added Show Comment Indicators in the model tree.

Good luck, Brian                  [original post 2020-02-13]  

P.S. Don't fear to edit the default tolerances for various uses.  You should have a different standard for sheet metal parts and CNC parts. If there are specs you use a lot... Instead of tons of separate templates it is easier to drop the Tolerance note into the Design Library. --> 1) Pin design library open. 2) Ctrl+C Copy the note from the drawing. 3) Ctrl+V paste into the design library, and a panel will pop up where you can name the note (make sure it is a .sldnotestl)  4) Later on drag in into your new drawing (while editing sheet format).