Drawing Templates versus Sheet Formats: What's The Difference?

This article clarifies the differences between drawing templates and sheet formats, and describes how to properly save each of these file types.

One of the most common technical support issues raised by SOLIDWORKS users is understanding the difference between drawing templates and sheet formats. Let's jump right in to first understanding what templates are.

SOLIDWORKS Templates

There are 3 main SOLIDWORKS file types; parts, assemblies, and drawings. A template is nothing more than bare versions of these file types where some settings have already been established.

The SOLIDWORKS Welcome screen, usually visible when first starting SOLIDWORKS, is one way of accessing templates. If the Welcome screen is not showing, click the "house" icon on the SOLIDWORKS title bar, or press Ctrl-F2.

The Part, Assembly, and Drawing icons on the Welcome screen are not the templates. It's necessary to click the Advanced button for those. Clicking Advanced will show the default Part, Assembly, and Drawing templates. As additional templates are created, they will be displayed with the original 3 that are already there.

Another method of viewing your templates is to click the New icon, or select New... from the File menu, or press Ctrl-N. If you're attempting this, but see the 3 big buttons that say Part, Assembly, and Drawing, click the "Advanced" button near the bottom left corner. If the button says "Novice", you're looking at your templates.

Since it is outside the scope of this article, we won't go into detail about how to create your own templates. However, the basic process involves these steps:

1. Start a new SOLIDWORKS document (part, assembly, or drawing).
2. Modify any of the settings found in the Tools menu > Options > Document Properties tab.
3. Click the File menu > Save As, and change the "Save as type" drop down menu to say Part Template, Assembly Template, or Drawing Template (depending on what you started out with).
4. Enter a name of your choosing and click the Save button.

Drawing Formats

Templates exist for every SOLIDWORKS document type, but sheet formats are strictly for drawings. Think of the drawing sheet format as the border, zones, and title block of a 2D drawing. A drawing can be a blank sheet of paper, or it can contain a format.

File Types

Now that it is understood that drawing templates and sheet formats each serve very different functions, it should come as no surprise they are also different file types. A drawing template has a file extension of .DRWDOT, whereas drawing sheet formats are .SLDDRT. 

Saving Sheet Formats

Saving sheet formats aren't accomplished with the Save As command. Instead, sheet formats have their own dedicated command in the File menu, aptly named Save Sheet Format.

Editing Sheet Formats

Sheet formats don't contain settings in the same way drawing templates do. Formats mostly consist of text and sketch lines. We won't get into the finer aspects of modifying formats in this article. To briefly summarize, any of the sketch tools can be used, along with the Note command, to get the format looking prim and proper.

Embedding Formats in Templates

As we learned earlier, drawing templates can contain sheet formats, or they can be blank sheets of paper. It's far more common to see a format included with a drawing template. Since there are different sheet sizes, there must also be different sheet formats to fit those sheet sizes.

Drafting Standards

There are default, or "canned" formats, to fit every standard sheet size. This is true regardless of which drafting standard is used (ANSI, ISO, etc.). When starting a new drawing, SOLIDWORKS will usually ask what size sheet should be used. This is accomplished via the Sheet Format/Size window, and is shown here.

Changing Drafting Standard

One of the things that can go wrong at this point is the drafting standard may not be correct. If the Sheet Format/Size window shows ISO sheet sizes (such as in the previous image), but your company uses the ANSI drafting standard, this would be a problem.

If this happens, cancel out of the Sheet Format/Size window, and access your SOLIDWORKS Options (that gear at the top of the SOLIDWORKS window). Click the Document Properties tab, and look for the Drafting Standard category, which should appear automatically. Pick the appropriate drafting standard from the drop down menu, then click OK to close the Options window.

Earlier, we briefly mentioned how anything modified in Document Properties will be saved in the template. Changing the Drafting Standard is a perfect example of this. If you want to make the change stick, the template needs to be saved. Refer back to the third step mentioned earlier if you need a reminder of how to do this.

The Format Path

Formats are files which are embedded in the drawing format. The term "embedded" is different than "linked". Embedded files will not automatically update if changes are made to the embedded file. The host file (template) does not maintain a live connection to the embedded file (the format). This plays a significant role, which we will explore in a moment.

To see what format has been used in a template, it is necessary to access the Properties of the drawing. There is a stumbling block you will likely run into when trying to access the drawing's Properties. Let's quickly explore this side topic.

The Hidden Properties

When right clicking on the drawing sheet, the right mouse button menu will appear. For reasons unknown, the Properties command was made absent from the default menu selection. Do yourself a favor and make it accessible. The process is simple. First, select the small double arrows at the bottom of the menu.

Next, select Customize Menu.

Finally, place a check in the checkbox to the left of Properties, and then click anywhere off the menu.

If you didn't already know how to customize menus, now you do. Additionally, the Properties command will now appear when right clicking on the sheet.

Back On The Path

Now that you know how to access a sheet's Properties, go ahead and do so. The path to the format will be shown to the left of the Browse button, and partially visible in the following image. Sometimes only the file name will be displayed without the full path. This is normal.

Occasionally, paths change for various reasons. Sometimes files are moved, or perhaps SOLIDWORKS is upgraded. The end result is the path specified in the sheet's Properties is different than where the sheet formats are actually located. When that is the case, a problem occurs when trying to add a second sheet to the drawing. If the path to the format is incorrect, the default format will be used. This may not be the same format shown on the first sheet!

The fix is easy. Click the Browse button shown in the previous image, select the desired format, and click Open. Click the Apply Changes button to lock in the path and close the Properties window. Finally, make it a point to save the drawing template, or locking in the format path will only benefit the current drawing.

Now you know the difference between SOLIDWORKS templates and formats, and how to work with them like a pro. Happy Modeling!