When you make changes to the Document Properties those changes only affect the active document. If you want to apply them to new Parts then open a new blank Part and make the desired changes. Go to File > Save, and choose Part Templates (*.prtdot) from the drop-down at "Save as type:".
Name the file appropriately and save. I described the process for saving a Part template, but it's the same for Assemblies and Drawings. Just choose the appropriate template type from the drop-down. I'd strongly suggest saving templates (and sheet formats, and weldment profiles,etc) somewhere other than the default location in the SolidWorks installation folder so you won't lose them if you upgrade to a newer version. If you're in a multi-user environment you might want to save them on a network so they're available for other users.
Next go to Tools > Options > System Options > File Locations > Document Templates.
Click on the "Add..." button, browse to the folder where you saved the template, and select it. I'd suggest deleting the default location that's there now, but that's up to you. Now when you start a new Part you should have the new template available to choose from. If you don't, and you see this...
...which only has the default templates to choose from, click on the "Advanced" button at lower left. Then it should look something like this:
You only see one Part and one Assembly template here because that's all I have saved. Depending on your needs you can certainly have more. Just name them appropriately so you know what you're choosing. If you have a large number of document templates you can add sub-folders at the location you're pointing to at File Locations > Document Templates, and these sub-folders will show up as tabs in the Advanced New Document dialog box. See above. "Templates" is my main folder that contains my most used templates, and "Other Drawings" is a sub-folder that contains some drawing templates that I rarely use but don't want to get rid of.
While I'm on the subject, occasionally someone will ask how to apply new Document Property settings to an existing document. You can open a document with the desired settings, go to Tools > Options > Document Properties > Drafting Standard, and select "Save to External File...". Save this standard, then open the model or drawing you want to update, go to the same location, choose "Load From External File...", and Browse to and select the desired saved standard. I haven't used this much, and have gotten mixed results when I did, but it's worth a shot. If you're in this situation I'd encourage you to go to Drafting standard refusing to change. Dimension Styles not loading in automatically and view font not changing. What am I doing wrong? . The first part doesn't pertain to the subject here, but about halfway down (starting with post #7) Dan Pihlaja entered the conversation with some good information.
For Drawings, another option is to open the existing Drawing, then start a new one with the new Template, and copy sheets from the existing document and paste them into the new one. This isn't a perfect procedure either, since it doesn't save all the Document Property settings, but it might work for you.