This blog article illustrates the differences between “sheet format” and “templates” in SOLIDWORKS and how to use them.
Your templates hold all of your settings in Tools > Options > Document Properties. For example: units, decimal places, etc. Templates need to be saved for Parts, Assemblies and Drawings. You can do this by setting all of your settings to how you want them, then go to File > Save As > “Part Template” (for parts). Once it is saved, and you start a new part you will see your template appear as a template to select.
Sheet formats only apply in drawings and applies to anything in your titleblock or your border. You can edit your sheet format, by right-clicking anywhere on the drawing and selecting the option for “Edit Sheet Format.” This turns everything in the titleblock blue. These are all editable choices that can be added or deleted the same way you would sketch in SOLIDWORKS. If you would like to have a company logo in your titleblock, this is where you would insert it.
Another thing you can do in your titleblock is add links to custom properties. These properties will pull in from the part such as weight, material, description, etc. To add a custom property link select the Note feature from the annotation tab and drop it where you would like the note to be.
Then in the far left side of SOLIDWORKS in the Property Manager select the option for “Link to Property.” This will then bring you to the Link to Property dialog box with a couple of choices. If you select “Current Document”, the property will pull from the custom properties in the drawing. If you select “Model in view specified in sheet properties” or “Component to which the annotation is attached” it will pull the custom properties from the part that is on the drawing sheet.
Once you have made your selection, use the drop down arrow to select what property you would like and hit ok.
You will know that the property linked correctly, if you hover over the note and see a dialogue box appear that looks like $PRPSHEET:”custom property specified” (see Figure 1).
Once you have the sheet format finished, exit the sheet format by right-clicking on the sheet and selecting Edit Sheet.
Lastly, we need to do a save. To do this please go to File > Save Sheet Format.
Ashley Johnson is an Application Engineer and a member of the technical staff at DASI Solutions, a SolidWorks Value Added Reseller with locations throughout Michigan and Indiana. She is a regular contributor to the DASI Solutions Blog.