i think i found it - i will try and let you know!
Stamping the Workflow State on SolidWorks Drawings in Enterprise PDM
Having a watermark on a SolidWorks drawing which indicates if the drawing is for production, prototyping or if the drawing is obsolete can assist in controlling documents that have been printed. Adding an annotation linked to a document property is a standard SolidWorks feature. Create a file property called “status” and add a note which contains the $PRP:”STATUS” syntax in the text.
Populating the file property value as a document transitions through the EPDM workflow is a little more involved. Here are the steps to follow:
1- Create a Variable named ‘Status’.
2- Map the Variable to a Custom Property Attribute which matches what the SolidWorks Drawing file will use for its annotation.
3- Decide where to stamp the variable in the documents workflow. For example if the drawings should be stamped “Prototype” then make sure the workflow has a Prototype state and a transition leading into that state.
4- Modify the transition that leads to the target state and add an Action.
5- Create a Set Variable action that sets the desired variable to %deststatus% (the destination status).
6- In some cases the variable may only need to be written to drawings. Adding the file extension to the ‘Only run for files with these extensions’ portion of the Transition Action will only stamp SLDDRW files. Only adding the SLDDRW file extension to the Variable Custom Property Attribute will have the same effect.
When a SLDDRW file transitions from ‘Waiting for Approval’ to ‘Prototype’ the variable will be written to the file and will appear on the SLDDRW file provided there is an annotation present to display the file property.
Create a note on your drawing template sheet format. Link the note to a custom property (call it Release Status or something). Link the custom property to an EPDM variable and manipulate the value of the variable via transition actions. For example, when the preliminary review transition happens, set the variable to 'NOT RELEASED'. When it passes approval, set the variable to a single space character.
I question the need for this giant note though. You already have NR in the title block. You shouldn't need to plaster 'NOT RELEASED' across the entire drawing. People should be trained to not work with drawings that do not have an actual revision number/letter.
Putting the revision/version (not sure what the point of having the version would be) in the BOM will require yet another variable linked to a custom property. In my setup, the variable is TB_REVISION (title block revision). It is linked to the revision annotation in my title block and it is kept synchronized with the EPDM file revision via transition actions. You can add a column to your BOM template that also points to this custom property.
There is one very big caveat when you put the revision of the parts on the BOM. If you don't have a formal ECO/ECN process, people will revise the part and not rebuild all the drawings of assemblies where the part is used. If you have generated PDFs, they will show the wrong revision for the revised parts compared to what you see when you open the SolidWorks drawing (the drawing will update when opened, even though you may not be able to save the changes). Until you open the drawing, rebuild it, save it and regenerate the PDF, things are out of whack.
We don't have a formal ECO/ECN process here, so to alleviate this problem, we don't put BOMs inside the drawing border. Thus the generated PDFs will not show bad data. So how do we see the BOMs? I wrote an add-in that lets users right click on an assembly model, assembly drawing or PDF of an assembly drawing and click 'Print BOM'. The add-in will compare the revisions of the parts in the EPDM BOM with the revision column of the SW BOM saved in the drawing and flag any items that don't match. The add-in then exports the BOM data into a nicely formatted Excel spreadsheet ready for printing. The items that don't match are bold and red so they stand out. Consumers of the BOMs know to contact Engineering when they see this so that we can update the assembly drawings.
I've been requested to add watermarks to drawings per states also. The process mentioned is the correct method. But, I did find a bug in it. When the drawing is opened in eDrawings, the watermark will be over the geometry and in black. I've notified my VAR, and he has placed in a fix request. It seems that eDrawings 2015 does not support this function, but eDrawings 2014 did.
What you will have to do in the meantime, is to notify your users when they print from eDrawings and/or the EDPM preview window, that they need to set the print color from black & white to color greyscale. This will lighten up the watermark, but will not place it behind the geometry.
I didn't see it mentioned above - Set the watermark text to be a Block. When you do that it sends the block to the back, and when creating a pdf or printing the dimensions should be on top. I'm not sure about eDrawings, but it may help.