Tools To Help Create SOLIDWORKS Sheet Formats

Article by Ray Morrogh updated March 7, 2024

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Using SOLIDWORKS sheet formats is how you can quickly update your drawing to change title blocks, table layouts, and add common annotations. Even though they are so foundational to your drawings, they are easy to edit and have a lot of great tools to achieve common formatting needs and incorporate custom properties. Here are some of the best tools to help you when creating new sheet formats.

SOLIDWORKS Sheet Formats: Automatic Borders

Automatic borders help create the borders of your drawing sheet in a way that can be easily edited. Adding and removing zones is just a single click away, and margins are easily controlled. This is much faster than manually adding all of this information. If you have legacy templates that are in a DXF/DWG file format and want to update those borders to be parametric, you can delete those entities on the first page of the command.

The second page of the command is where you’ll create your border, and the third page is where you can insert a margin mask. This is an opportunity to block out some of the borders you just made to insert a link to a custom property that may be too long to fit in your title block like a file location.

Automatic Borders in Sheet Formats

When editing your sheet format, right click on the sheet format drop down to access the “Automatic Border” command.

SOLIDWORKS Sheet Formats: Title Block Fields Wizard

Linking custom properties to a title block field is a great way to ensure that text automatically populates with the right information. What if you want to make quick changes though? Navigating to the properties, finding that property, and changing it can be tedious, but the title block wizard makes it a snap. You can even edit text that isn’t linked to a custom property without having to go in and edit the title block.

Title Block Wizard

Right click “Sheet Formats” and click on Title Block Fields to start the Title Block wizard

This command will ask you to put a bounding box around the area where you’d like to select text. Then simply selecting editable text fields (Again, this doesn’t have to be properties. Select millimeters or tolerance values to directly edit them) and selecting check will make it so that when you exit the sheet format editor, you can double-click on any text field you selected to directly edit it. This bi-directionally connects to the intended property too, so edits made here will show up in your properties and vice versa, making it a snap to edit those custom value fields.

 

SOLIDWORKS Sheet Formats: Center in Box

Right-clicking any note inside your title block gives you an option called “Center in Box”. Clicking this option may not look like it does anything at first, but selecting four perpendicular lines will center your annotation in its box. One great thing to know here is that line lengths don’t matter; SOLIDWORKS is centering the annotation in the box that is the intersection of those four lines.

SOLIDWORKS Sheet Formats: Select on Open

If your company uses a wide variety of functions within SOLIDWORKS, you may have different sheet formats depending on what you are trying to represent. Different title blocks or layouts for parts, assemblies, weldments, and sheet metal parts may make a lot of sense for your company’s communication with the shop floor. Rather than having the same default format for every drawing, you can actually save your drawing template (.drwdot) without a sheet format (.slddrt). This gives you the freedom to choose your sheet format every time you start a new drawing, a nice time saver if you find yourself typically having to navigate to the properties of the sheet format to change the .slddrt file you are referencing.

Something else to note if you’re doing multiple sheets in drawings, is that there is a setting within your drawings document where you can have a default sheet format for additional sheets. Navigate to document properties and then to drawing sheets to find the area to input that file location.

Sheets Drawing Properties

Check the box up top and browse to the .slddrt sheet format file you’d like to default to for added pages

Interested in just ditching drawings altogether and communicating to your shop floor with your 3D Models? Check out SOLIDWORKS MBD.

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Ray Morrogh

Ray Morrogh has been using SOLIDWORKS since his graduation from Virginia Tech in 2018, where he studied Mechanical Engineering with minors in Physics and Industrial Design. A recent addition to the TriMech team, he previously worked in consumer packaged goods and product development, creating everything from power tools to footwear to kitchen products. He has a passion for great design and loves seeing how people use SOLIDWORKS to bring their visions to life.