SOLIDWORKS Tutorial: Step-by-Step Guide to Drawing Templates and Sheet Formats [VIDEO]

Article by Scott Durksen, CSWE, last updated on February 16, 2018

Many people get confused when it comes to creating custom Drawing Templates and Sheet Formats in SOLIDWORKS.  It’s not as straight forward as Part and Assembly templates due to the fact that each sheet can potentially have different sheet sizes and title blocks.  Because of this extra detail, the information is broken out into two files.  Understanding what information is contained in each file and how they interact with each other is important to create a proper drawing template.

What’s contained in each drawing file?

Drawing Template File (.drwdot):
  • All settings under Tools > Options > Document Properties tab
  • All existing sheets
  • All sheet formats on existing sheets
  • All existing predefined views
  • Link to Sheet Format file specified in Sheet Properties (right-click on sheet > Properties)
Sheet Format File (.slddrt):
  • All information stored in Sheet Format (right-click on sheet > Edit Sheet Format); this includes borders, titleblocks, logos, etc.
  • All table anchors (BOM, Weldment Cutlist, etc)

As mentioned in the Drawing Template file, any existing sheet in the template already contains a Sheet Format.  However whenever a new sheet is added, it references the Sheet Format link that is specified in the active sheet properties.  This is why a saved out Sheet Format with a link in the Drawing Template is key, otherwise you will receive the error “The sheet format could not be located”.

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How to create a Drawing Template linked to a Sheet Format file

  1. Start a blank new drawing via File > New
  2. Edit the Sheet Properties (right-click on drawing > Properties) and choose the sheet size (A, B, C, etc), set the Sheet Scale, etc.  Click OK.
  3. Edit the Sheet Format (right-click on drawing > Edit Sheet Format) and customize the titleblock, border and anchors
  4. Accept the changes and return to the Sheet via the Confirmation Corner (top right of the graphics area)
  5. Save the Sheet Format file by going to File > Save Sheet format.  This will save an .slddrt file.  It’s recommended to save this in a custom location that is easy to find.  This path can be specified under Tools > Options > System Options tab > File Locations > Sheet Formats.
  6. Return to the sheet Properties (right-click on drawing > Properties), and choose to Browse for the Sheet Format.  Select the .slddrt file that you just saved.
  7. Edit any other Sheet Properties (Type of Projection, Sheet Scale, etc) and click OK
  8. Add any predefined views as needed
  9. Go to File > Save As and choose to save as the Drawing Template (.drwdot) filetype.  Save in a custom location that is easy to find.  This path can be specified under Tools > Options > System Options tab > File Locations > Templates.

Scott Durksen, CSWE

Scott is a SOLIDWORKS Elite Applications Engineer and is based in our Dartmouth, Nova Scotia office.

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