CAD Forum

Those changes only affect the active document. If you want them to be reflected in new documents you will need to open a new document, make your changes, then go to Save as and choose "Drawing Template" (or Part Template, or Assembly Template) from the drop-down.

I'd suggest saving custom templates in a location other than the default so you don't lose them when you upgrade to a new version of Solidworks. If you're the only user save them somewhere else on your hard drive. If you're in a multiple user environment you might want to save them on a network drive (or cloud location, whichever is appropriate) so other users can access them, and to maintain consistency within the company.

Be sure to point to the location where you saved the template(s) at Tools > Options > System Options > File Locations > Document Templates. If you have custom templates for each file type it's okay to delete the default location from the list.



Now, when you start a new document, if you don't see your custom templates choose the "Advanced" button . . .


. . . which will take you to a different new document window.


As you can see, I only have one Part and Assembly template, because that's all I need, but you can have more if you need to. I do have multiple drawing templates. You might also notice that there is a second tab, "Other Drawings", that doesn't appear for you. I have some templates that I rarely use, but don't want to get rid of, and didn't want them cluttering up the main list, so I put them in a sub-folder in the folder with my main templates. Each sub-folder in the folder you're pointing to at File Locations will add another tab. If you have multiple clients, and have templates for each, this might be helpful.

it's also important to know, and to use the commun name for : DOT (to avoid mistake with sheet-template)

DOT for PRT (extention file = prtdot)
DOT for ASM (extention file = asmdot)
DOT for DRW (extention file = drwdot)

and to simplify, when the user does "File / New"
Solidworks use the DOT to create the new file.

Must be careful when exporting documents properties for drawings, half of them are NOT saved and must be manually added later. Easy to lose them when upgrading SW and making new templates from scratch. As per KB

Question
Are all document settings ('Tools > Options > Document Properties') included in the 'Drafting Standard' file (.sldstd) when it is exported?

Answer
No. The file exported as the drafting standard file (.sldstd) contains some of the document properties and not all settings. Settings like dimension, annotations, tables etc., are included in it and other settings like units, line font, image quality etc., are not included in it. Refer to the attached image showing the customizable standards which can be included in ‘Drafting Standard file.’

In general, the settings under ‘Document Properties’ ('Tools > Options') are saved in the document (part, assembly, drawing) template but when the user wants to modify some specific settings, they can change it in "Document Properties".

If the settings that the user is changing for any particular file are also applicable for other documents, in order to simplify the user’s tasks SOLIDWORKS® has provided the option to import/export ‘Drafting Standards’. These drafting standards can then be loaded into another SOLIDWORKS document to apply those (previously modified) settings to that document.

QA00000117239