Every company that is new to SOLIDWORKS has similar issues to tackle when they are first getting started with the software. Here are some of the most common questions we receive from clients: 

• ”How can I utilize my legacy CAD data in this new program?”
• “How can I get my engineers started in designing as soon as possible?”
• “How can I create a drawing that contains my company’s specific title block and automatically adheres to our standards?” 

SOLIDWORKS comes with a number of generic out-of-the-box title blocks that can be tweaked and customized to any new client’s liking. However, if you already have a specific format that you like your drawings to follow, there are other ways to utilize that data in setting up your SOLIDWORKS Drawing Templates. This is especially useful if you already have drawings saved in a DXF or DWG file format. 

This is something that is fairly easy to do, but it requires a little background information in order to fully understand the approach one should take. The first important distinction to make is the difference between a Drawing Template and a Sheet Format in SOLIDWORKS. 

Drawing Templates

Your Drawing Template, much like your Part and Assembly templates, is the specific set of standards used in drawing and dimensioning your part. The answers to questions such as “What default font is used?”, “How many decimal places are used?”, and “What do my leaders look like?” are all specified in your Document Properties. To set up your Document Properties for a drawing, open a drawing and go to Tools > Options, and switch to the Document Properties tab. When all options are set to your liking, you can save these properties into a drawing template that can be accessed whenever a new drawing is started. To save a drawing template, simply go to File > Save As and change the file format from Drawing (.slddrw) to Drawing Template (.drwdot). 

Other than the settings found under Document Properties, there are certain sheet properties that can be saved to your Drawing Template. You can access these properties by right clicking anywhere in the blank space of a drawing and choosing Properties. Your Sheet Properties dialogue contains information such as the default view scale and whether you are using first or third angle projection. It also contains the link to your  Sheet Format. 

Sheet Formats

Your Sheet Format represents the physical piece of paper that the drawing is placed on, including sheet size, border and title block information. Because many times a specific Sheet Format is saved into a Drawing Template, many people aren’t entirely sure of the difference. However, they are indeed two entirely different things. 

Sheet Formats are edited by right clicking anywhere in the blank space of a drawing and choosing “Edit Sheet Format”. You may notice that you are now able to click and drag any lines that are not fixed in place (these are essentially sketch lines). You can move, add or take away lines, add images such as a company logo and also edit the notes that are part of the sheet format, including the ones that state part name, part number, revision number etc. 

When you are finished adjusting your Sheet Format, you can right-click again in any blank space on the drawing and choose “Edit Sheet”, which will return you to the regular drawing environment. Your title block and border will no longer be editable. In order to save your customized sheet format you can go to the file menu, but instead of choosing “Save” or “Save As…”, you should select “Save Sheet Format”. This will save this Sheet Format as a .slddrt file. This sheet format can now be accessed by multiple different drawing templates.

Sheet formats can also leverage file properties from your part and assembly models to auto-populate fields for the title block, such as Part Number, Description and Material, making them very useful when set up correctly. If you do not wish to start from scratch or use one of the standard sheet formats included in your SOLIDWORKS installation, another option is to import a title block from a DXF or DWG file. This allows you to reuse original 2D drawing data and quickly configure drawings tailored to your specific needs.

For more information on templates in SOLIDWORKS, view our four-part webinar series, SOLIDWORKS Templates 101.