Drawing borders can be created using standard sketch geometry, or using an automated function. This article shows how to use the Automatic Border command.
There are often easier ways to accomplish tedious tasks in SOLIDWORKS. The Automatic Border command falls into this category. It is not necessary to create sketch geometry using various sketch tools to draw a border on a drawing sheet.
The Automatic Border command can be found on the Sheet Format tab of the CommandManager. For the command to be available, a SOLIDWORKS drawing must be opened, and you must be editing the sheet format.
Automatic Border is a command that debuted with the release of SOLIDWORKS 2016. If your drawing templates are still using standard sketch geometry for their borders, it is an indication the template may be older than 2016. Bringing old templates forward year after year is convenient, but not a good idea.
Old templates can introduce odd behavior in SOLIDWORKS files. This can manifest in a wide assortment of symptoms. Old templates also may be lacking in functionality, such as missing anchor points for various tables. It's best to recreate templates from scratch every 3-5 years.
Using The Automatic Border Command
Let's walk through an example of using the Automatic Border command. We will be making changes to a stock ANSI A size drawing template, shown in the next image.
Automatic Border: Page 1
The Automatic Border command has 3 pages. Page 1 allows for selecting any entities that should be deleted. This is convenient if there is an existing border with title block. The sketch entities and zone labels making up the border can be deleted. The title block area can remain, as it will still be useful. If there is nothing to delete, just click the Next arrow.
Automatic Border: Settings
The second page may seem intimidating at first, but most of the settings are self-explanatory and straightforward. Experiment with the various settings to see how they affect the border. Everything updates immediately, so it's easy to observe what happens when tweaking the settings.
After making a few adjustments, our border is coming along nicely.
Automatic Border: Masking
The third and final page is for masking. Specifically, masking (hiding) any portion of the border that should not be shown. An example where this would be useful is if a company logo was occupying the same area as a portion of the border or zone labels. In such a case, the mask could be used to hide the border so it would not appear over the logo.
Creating a mask, if needed, is done by clicking the plus sigh button shown in the image below. A grey rectangle will appear. The rectangle can be dragged to reposition it, and the corners can be dragged to resize the rectangle. Click the green check to complete the Automatic Border command. If a mask was used, whatever portion of the border that was behind the mask, including the zone labels, will be hidden.
Good practice is to mask the title block region. Try to do this without going over the border. This will keep any zone divider marks from infringing on text in the title block. Zooming in close to the bottom right corner will aid in positioning the mask.
Title Block Final Steps
Now that the border is finished, it may be necessary to reposition the title block. This will almost certainly be necessary if the border itself has been repositioned.
The easiest way to move the title block (assuming it is not an actual block entity), is to use the Move command, which can be found in the Tools > Sketch Tools menu. After invoking the Move command, use the standard rectangle selection technique to select all of the entities in the title block.
The "From/To" option seems easiest. A random point in an empty area can be selected as the "from" location, and the cursor (mouse) can be moved to locate where the title block should go. This may take a couple tries, depending on how precise you want to be. Zooming in on one of the endpoints of the title block geometry will make this task easier.
If snapping gets in the way, hold down the Ctrl key to temporarily disable it. This allows for "eye-balling" placement of the title block.
Don't Forget To Save!
Considering we've just modified the sheet format, it would be a good idea to save it. Assuming you're using desktop SOLIDWORKS, click the File menu > Save Sheet Format to accomplish this task. You should also save the drawing template. This can be done with the File > Save As command.
Have we forgotten anything? Maybe. It depends on whether a new name or path was given to the sheet format. Access the properties of the drawing sheet via the right mouse button menu and set the path for where the format is located.
If the path did need to be re-established, save the template again to make that setting stick. Now your work is done.
Happy modeling!