Creating SOLIDWORKS Drawing Templates with Enterprise PDM

The process of creating a SOLIDWORKS drawing template seems to be very lacking in the amount of training resources available. I would like to take some time to explain how the main components work together and show some best practices for creating and configuring your SOLIDWORKS templates.

The first component is what I refer to as the DOT file, and is the base template that you will use for your files. This file is where you can configure various settings about the file that will be created, such as the paper size, dimensioning styles, hatch patterns, etc. (most everything under Tools > Options). To create a SOLIDWORKS part or assembly template is easy. Simply open a new document, (you can use an existing template if you would like), modify the options that you would like to change, then go to File > Save As and change the file type to the DOT extension. The extension is different for each file type, for instance, a SOLIDWORKS part file will have a .prtdot extension, while an assembly and drawing file will have a .asmdot and .drwdot extension respectively. Also notice that the save location will change based on where you have the file template location set up in SOLIDWORKS.

Once saved, you should see your new template file during the template selection when creating a new file. If you are creating a template for a SOLIDWORKS part or assembly, then the DOT file should be all that you need. However if you are putting a SOLIDWORKS drawing template together, then you will need the second component that I refer to as the DART file. The DART file is file extension .sldDRT and is the actual sheet format for any drawing that you may be creating. When referencing the two different file types, it’s helpful to imagine a dart board. Imagine the board and it’s bulls eye as the DOT file, then the DART file get’s placed into it. Once you have created your basic DOT template for your drawing, it is time to create the new sheet format that will be used (the DART file).

For drawings, it is much easier to create both the DOT file and the DART file at the same time. We also recommend using some of the standard drawing sizes and title blocks that are available so there is no need to start from scratch. Start by creating a new drawing and choosing a sheet format that closely resembles your sheet size. Choosing “Edit Sheet Format” by right-clicking in an open area will allow you to modify the borders and title blocks inside of the drawing using the standard SOLIDWORKS drawing utilities.

You will now see a button in the top right corner indicating that you are editing the sheet format.

At this point you are free to make any modifications to the title block and text. It is much easier to put any standard notes and text into the sheet format so you are certain that each new drawing will contain the necessary information, such as text that is linked to certain properties. To create a linked text, create a new text line by selecting “Annotation” > “Note” or “Insert” > “Annotations” > “Note”. After you have placed the note in the proper location, select the “Link to Property” option in the Note properties under the section “Text Format”.

There are multiple ways to link the text to a property:

1. Current Document
   1. Link this text to one of this drawing files custom properties.
2. Model in view to which the annotation is attached.
   1. If the note is inside of a model view, it can utilized that models properties.
3. Model in view specified in sheet properties.
   1. Link this text to one of the main models properties. This is typically the first model view imported, but can be changed in the sheet properties.
4. Component to which the annotation is attached
   1. If this note is pointing to a specific part, it can utilize its properties or it’s cut list properties.

Depending on which type of link you select, there will be a different placeholder syntax for that note;

1. $PRP:{Property}
   1. Looking at the current document property.
2. $PRPSHEET:{Property}
   1. Looking at the referenced model property.

Once the borders, title block and notes are set up inside of your sheet format, make sure to exit the sheet format editor by clicking the button in the upper right corner, then save it by going to “File” > “Save Sheet Format…”. The Save As directory will automatically point to the location that is referenced in your SOLIDWORKS options and the extension will be set to .slddrt.

After the sheet format (or DART file) is saved, save the new template (or DOT file) as well. In a nutshell, you’ve created a border, title block and notes, and now you are saving a template that will always use that format.

Working with SOLIDWORKS Enterprise PDM

If you are working with SOLIDWORKS Enterprise PDM, then there may be some additional things that you need to be aware of before pushing these drawing templates onto the users. The first thing to remember is the EPDM data cards are typically set up to look at their own files properties. If your drawing is using only linked variables that are pulling from the referenced model, the drawing will have no properties of its own, thus it’s data card will not populate as it has nothing to read. We will need to modify the attributes in the EPDM variables to work around this.

Inside of the Enterprise PDM Administration tool, log into your production vault and open up your SOLIDWORKS drawing file data card.

For each variable that you would like the data card to read from the drawing file, you will need to adjust those variable attributes accordingly. To put it shortly, the attributes are what a variable looks for inside of its file. Clicking on the “Variables” button in the top right will open the “Edit Variables” window.

For each variable that will be associated with a SOLIDWORKS drawing file, you must ensure that it has at least two attributes with the slddrw extension;

1. CustomProperty
   1. Looks for the file’s custom property.
2. $PRPSHEET
   1. Looks for a linked note in the SOLIDWORKS drawing file.

This ensures that when the data card is attached to the SOLIDWORKS drawing file, it can see the note that is placed into the drawings title block, then transfer that to the drawings custom property as well!

If you need more assistance or have questions, please contact Inflow Technology Support at 888-285-2285 or at support@inflow-tech.com .

Derek M. Lawson – PLM Consultant