Every company that is new to SolidWorks has similar issues to tackle when they are first getting started with the software: ”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?” One of the most common questions we get from new SolidWorks customers is “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 customer’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 specifically 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 one must make is the difference between a drawing template and a sheet format in SolidWorks.
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 setup 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 (.slddot).
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.
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.
If you do not wish to start from one of the standard sheet formats SolidWorks provides, but would rather assign your own sheet format, you can import a title block from a DXF or DWG file and then set up your linked notes as described above. In order to do this, simply go to File > Open as if you are opening any SolidWorks part file. Browse to the appropriate DXF/DWG file and open it. You will be prompted with some options, since SolidWorks recognizes that you are attempting to open a 2-dimensional file in a 3-dimensional environment.
1) First choose to create a new SolidWorks drawing and convert to SolidWorks entities. Then hit next.
2) In the upper left corner of the next window choose to show “layers selected for sheet format” and then check off all layers that contain entities you would want as part of your border and title block in your new sheet format. Remember, you can always edit and delete some entities after the fact. When you are done, choose next.
3) The third page allows you to set your units and paper size, as well as choose where the title block will be located on the sheet. You should choose for it to be centered. Now when you click “Finish” SolidWorks opens up a drawing file with your old title block as the sheet format.
You can edit this sheet format and save it as a standard one as outline above. For more detailed information on customizing sheet formats, setting up custom properties to link to notes and creating all sorts of document templates, including drawing templates, you should watch this one hour webinar hosted by CAPINC’s own Crystal Yazvac. In it, she walks you through many different procedures needed to set up and edit your own company standards, templates and title blocks.