The set of standards used for drawing and dimensioning your parts in SOLIDWORKS is known as the Drawing Template, similar to Part and Assembly templates. SOLIDWORKS drawings consist of two distinct layers, the sheet and sheet format. These both make up the drawing template. In addition, any changes you’ve made to the Document Properties will also carry over to the drawing template once that template is saved. The drawing template, sheet and sheet format all combine to make up the drawing file (*.slddrw). In this blog article, we show you how to set up your Drawing template.
The Sheet and Sheet Format
The sheet is where all the views of your part or assembly will reside. Any dimensions, annotations or other markup also reside on the sheet.
The sheet format (*.slddrt) contains the border, title block, sheet size and some other items. The sheet format can be edited to customize these items and match our company standards.
There are a few ways to edit the sheet format. Introduced in SOLIDWORKS 2016, there is now a Sheet Format tab with an Edit Sheet Format button. This is the same functionality as right-clicking anywhere on your drawing and selecting Edit Sheet Format from the right click menu.
Once you’re finished making changes, you can click the Edit Sheet Format button again on the Sheet Format tab or right-click on any blank space and choose Edit Sheet. Save the changes you’ve made to a sheet format file by going to File > Save Sheet Format.
To better illustrate these two default layers, here’s a page from the Drawings training class:
SOLIDWORKS Drawing Templates
A drawing template serves as the starting point for creating a drawing. The template typically references a specific sheet format file. If we want to see which sheet format file is being referenced or change it to a different sheet format file, we can do so by right-clicking on the sheet in the drawing tree and choosing Properties.
You can choose a new sheet format file by clicking Browse. Some customers prefer a different border and title block on their second or third drawing sheets. You can set sheet properties, including sheet formats and zone parameters, for multiple drawing sheets at the same time using the Select Sheets to Modify button introduced in SOLIDWORKS 2017. The drawing template is like the SOLIDWORKS part and assembly templates, where it captures the settings you set in the Document Properties tab in the Tools > Options box.
Some common settings to control include the drawing’s units, font styles and sizes and dimension precision. Some new examples include how to handle trailing zeroes for dimensions, properties and tolerances and setting All Upper Case Characters for tables. The drawing templates are usually shown when you choose File > New in SOLIDWORKS. You might notice that there are several different tabs displayed when you choose to start a new drawing.
These tabs correspond to different folders listed within your document template settings. These can be set by choosing Tools > Options > System Options tab > File Locations. For an organization that wishes to share templates among their employees, it makes sense to store these document template files on a network drive or within the SOLIDWORKS PDM vault.
To create a new template, or modify an existing one, the process typically goes something like this:
- File > Open and change your file type option to Template. To create a new template, open a preexisting template from the SOLIDWORKS installation or open a drawing file (slddrw).
- Change the drawing sheet size if necessary.
- Change the sheet format to the desired sheet format file.
- Change any options needed within the Document Properties.
- Save the template file to one of the locations listed within your File Locations in your System Options.