Tag: watermark

Sometimes it’s the little new things (~part II) in SolidWorks 2013: Watermarking

This entry is part 7 of 12 in the series New in SolidWorks 2013

There’s been a long trail of discussions on the topic of adding watermarks to SolidWorks drawings.   For one reason or another, watermarks are seen by some as necessary in drawings.  The starting point of the conversion can be roughly traced back to the SolidWorks Forum in 2006.   In December 2007, I did one article that incompletely addressed the need.  If you just needed text to show up on your sheet format, you can review the first article.

Then, a question was asked at the first Stump the Chumps presentation at SolidWorks World 2008 about how to add watermarks to drawings.  No answer was given at that presentation (the chumps where stumped).

Soon after SolidWorks World 2008, Ben Eadie (one of the stumped chumps) found an About SolidWorks article that discussed various aspects of this topic.  (The article appears to have been maintained/updated since then.)     Around that time, I also wrote a detailed article about how to link your custom properties to your watermark and provided a trick  to get the watermark note to appear underneath elements on the drawing sheet.  Linking custom properties to the watermark allows the watermark value to be controlled by Enterprise PDM workflows.

OK, so what was the trick to getting notes to appear underneath drawing elements? If you created a block of an annotation note on your sheet format, that note block will appear under your drawing (without obscuring drawing content).

In Solidworks 2013, you no longer need to use that trick to get your sheet format note to appear underneath drawing elements.  There is now a command that resides in the right-click menu for each annotation note on the sheet format called “Display Note Behind Sheet”.  When checked, the  note is placed underneath drawing view elements on the drawing sheet, including other annotations, dimensions and model geometry in both HLR/HLV and shaded modes.

Display Note Behind Sheet is a checkmarked command in the
right-click menu for any annotation note on the sheet format.
.




With the checkmark set on the note in sheet format, the


note appears under all drawing view elements.


.




Uncheckmarking the option will apply standard ordering


of drawing elements, with geometry obsured by


the note.



	


	





	

		
		
How to add Watermark to SolidWorks Drawing (with linked value)
	


	
	
	

		
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.


Layer Toolbar


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.


Layer Window


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.


Annotation Note Properties Window


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.

	


	





	

		
		
Create a SolidWorks Drawing Watermark
	


	
	
	

		
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 drawing entities, a workaround is necessary. Here’s a method I recently discovered.(I am currently using SolidWorks 2007 SP3.1.)


 


    

  1. Open the drawing.
    2. 

  2. Edit Sheet Format
    3. 

  3. Use Annotation Note to create and place the text that will become the watermark. 
    4. 

  4. Edit the properties of the Note to adjust its font, angle, size, etc as desired.
    5. 

  5. Highlight the Note and change its color using the Line Color function.For best results, assign a very light color to the Note.
    6. 

  6. Right Mouse Button click on the Note and select Make Block and accept.
    7. 

  7. Edit Sheet.
    8. 



 


The Note will now appear underneath all other objects on the Drawing Sheet. This tip is based on the SolidWorks Forum discussion which can be found here:http://forum.solidworks.com/forum/messageview.cfm?catid=6&threadid=1989&enterthread=y


*UPDATE*


I have written an article detailing a more advanced method that will link the text of the watermark directly to a custom property here: Create a SolidWorks Drawing Watermark (with linked value).


>


UPDATE for SolidWorks 2013



SolidWorks 2013 now has the ability to set any annotation note on the sheet format to appear underneath all drawing elements to act as a watermark.  The method mentioned above is no longer necessary to achieve the desired results. Please see SolidWorks 2013 What’s New – Display Note Behind Sheet.