How do you automate watermarks through SOLIDWORKS PDM?

This article demonstrates and describes how to automate watermark creation on SOLIDWORKS drawing files using a workflow in SOLIDWORKS PDM.


Engineers often require a watermark on the SOLIDWORKS drawing to identify the state of the file like "RELEASED" or "NOT FOR PRODUCTION". Engineers many decades ago drew their designs using tools like a drawing board, pencils, vellum paper, and T-squares. Designers would use a rubber stamp and often red ink to clearly mark the drawing. Those were the good old days. 

Currently SOLIDWORKS PDM software can automate the watermark process through the workflow and thus standardize when the action happens for specific CAD drawings. The basic process applies to both Draftsight and SOLIDWORKS, but this blog will focus more on SOLIDWORKS drawings. 


Workflow State - Refer to Figure A below. A workflow state is recognized as a block on the flow diagram. Each state represents a point or stage of the document process that controls what can be done with that document and by who.

Workflow Transition - Refer to Figure A below. A transition is identifiable as an arrow on the workflow. Each transition enables the user to get from one state to the next. When a person chooses to change state in SOLIDWORKS PDM, the names of the transitions are shown as options.

Variable - A variable in SOLIDWORKS PDM identifies and captures the data from user input into the data card. In other words, it's a definition of the space in the database where a specific piece of data is stored and a user control on the data card is attached to it. 

Figure A.

SOLIDWORKS PDM Configuration

This section is broken down into two parts: data card and workflow. The workflow is the mechanism for inputting the data on the data card. On the other hand, the data card captures the data and transfers it to the custom properties of the associated file.

Data Card

Must have administrative permissions for "Can update variables" and folder permission for "Can update the design of cards". 

  1. Right-mouse-click on the "Variables" node in the SOLIDWORKS PDM administration tool and choose "New Variable...". 
  2. Create a variable in SOLIDWORKS PDM named "Watermark". See figure B below.

    Figure B.

  3. Set the "Variable type" to "Text".
  4. Choose block name "CustomProperty".
  5. Set the attribute name to "Watermark"
  6. Enter "slddrw, drw" for file extensions.
  7. Open the file card for SOLIDWORKS drawing files.
  8. Setup watermark control on the file data card.
    Refer to figure C below. 
    1. Choose "Edit" control from the top toolbar.
    2. Insert "Edit" control and size.
    3. Select "Watermark" for variable in the property pane to the right. 
    4. Finalize remaining properties for "Edit" control per figure.

The attribute name and the variable name are not required to match. The attribute name is the name of the custom property created in the associated file. 

Figure C.

Pro Tip - Hiding controls on data card.

Create a tab control on the file data card. Go to the last tab name in sequence and click the "<Enter>" key.  Do not enter a name. The tab will appear blank. Any controls added to this tab will not be visible to the user. 


  1. Choose a workflow and associated transition whereby the watermark value will be updated from. For this example, a workflow transition named "Release Documents" going to the state "Released for Production" will be used. See figure D below.

    Figure D.
  2. Double click on the chosen transition.
  3. Set properties per figure E below.

    Figure E.

    1. Click the "Actions" tab.
    2. Enter a description for the action which will appear under the associated tab.
    3. Select "Set Variable" from the droplist control for type.
    4. Choose "Run for files" and enter "slddrw" because this is the only file type watermarks are generally useful for. 
    5. Select "Watermark" from the droplist control for variable.
    6. Set value for watermark variable. For this example, "RELEASED" is entered. 

SOLIDWORKS Drawing Configuration

  1. Open SOLIDWORKS application.
  2. Open or create a new drawing template.
  3. Click "File" from the top toolbar.
  4. Choose "Properties" from the "File" menu.
  5. Add a new custom property called "Watermark" and leave the value empty. The workflow transition action will update it.  See figure F below.

    Figure F.
  6. Click "Insert" from the top toolbar.
  7. Choose "Annotations" and "Note..." menu items as shown in figure G below.
  8. Select a location for the annotation somewhere on the drawing sheet and format style accordingly. See figure G below.

    Figure G.
  9. While the note is selected, go to the property manager on the left-side of the screen. 
  10. Click the "Link to Property" button under "Text Format" section.  See figure H below.

    Figure H.
  11. Configure the link to property as shown in figure I below.

    Figure I.
    1. Use custom properties from "Current document".
    2. Select "Current Document" from the droplist.
    3. Choose "Watermark" property name. 
    4. Save drawing template.

Pro Tip

Consider formatting the note with a larger than normal font size and choose a different text color for more visibility. 

Pro Tip

Put the note on the sheet rather than the sheet format.  This suggestion enables the user to position the watermark more easily after it's updated automatically using SOLIDWORKS PDM. Moreover, one can position the note directly over a drawing view. This practice is often performed for watermarks that appear with "NOT FOR PRODUCTION" text. 

Pro Tip

Update the watermark through the workflow before file is transitioned to a state whereby it is made "Read-Only".  This action enables someone to reposition the watermark, if necessary.