How to add a Watermark to SolidWorks Drawings
By Matthew Lorono
For whatever reason, watermarks are sometimes necessary, even on drawings. Since SolidWorks has no watermark feature, and does not allow the user to change the order of certain drawing entities, a workaround is necessary. Here the most effective and powerful method useful for Drawing Templates and Sheet Formats.
1. Open the drawing.
2. Create a drawing layer by choosing the layer icon.
3. Change the layer name and description to something identifiable.Then click on the color block in the Color column and choose a very light color.Select OK.
4. Goto pulldown menu File and select Properties.
5. Add the property Watermark.As a place holder, give this property the value of “PRELIMINARY” or something similar.
6. Edit Sheet Format.
7. Use Annotation Note to create and place the entity that will become the watermark.
8. Edit the properties of that Note to adjust its font, angle, size, etc as desired.Then, link the Note to the custom property Watermark, as shown in the figure.Select OK.
8. Change the layer of the Note to the newly created layer.
**UPDATE: New functionality in SolidWorks 2013 makes steps 9 and 9.5 no longer necessary, please see this article for details: Sometimes it’s the little new things – Watermarking **
9. Right Mouse Button click on the Note and select Make Block and accept.
9.5. Due to some funky behavior that I’ve discovered by SolidWorks when loading a watermarked template into an existing drawing, I’m adding this one step: Once you make the block, change the layer of the block to the same layer you set for your Note.
10. Save the Sheet Format (under pulldown menu File and select Save Sheet Format).
11. Edit Sheet.The Note will now appear underneath all other objects on the Drawing Sheet.
12. Save this document as a Drawing Template (under pulldown menu File and select “Save As”, then change Save as type to “Drawing Templates”).This creates both the Drawing Template and Sheet Format with an embedded watermark.To change the text of the watermark in any drawings that use the Drawing Template, simply go back to Files>Properties, and edit its text value.To remove the watermark, simply replace the current value with a space.These instructions are geared towards SolidWorks 2007 or earlier. SolidWorks 2008 or later instructions will be similar, though how to access some of the functions may have changed.