Watermark or Stamp

[brojack17]

I would like to put a watermark or a stamp on a drawing that shows "Released" if the model parameter "PTC_WM_LIFECYCLE_STATE" = RELEASED. I do not want a stamp for any other lifecycle state.

I am using WC 9.1 and WF 5.

 

[mjk4134]

1) Add a parameter to the drawing "REL_STATUS"


2) Create a relationship for Rel_status as you would do for a bulk item in a bom
IF PTC_WM_LIFECYCLE_STATE = "RELEASED"
REL_STATUS="RELEASED"
ELSE
REL_STATUS=" "

thenplace the note: &REL_STATUS

If you want all status to show just enter a note with :
&PTC_WM_LIFECYCLE_STATE

 

[brojack17]

Thanks. It was the quote around the status that I was missing.

 

[jsantangelo]

This is nice and simple solution. We are going to give this a try for our drawings.

 

[brojack17]

I had to put the double equal sign in the IF statement

IF PTC_WM_LIFECYCLE_STATE == "RELEASED"

 

[Jase]

Im kinda new to Pro-E and am using WF3.0. Ive been set some tasks for my client and Im attempting the above in WF3.0 to watermark all non-Released Drawings with "FOR INFORMATION ONLY" but I keep getting a Relation error on the statement:-


IF PTC_WM_LIFECYCLE_STATE == "RELEASED"
REL_STATUS = " "
ELSE
REL_STATUS = "FOR INFORMATION ONLY"


Anyone got any ideas?


Jase
Edited by: Jase

 

[jsantangelo]

Im kinda new to Pro-E and am using WF3.0. Ive been set some tasks for my client and Im attempting the above in WF3.0 to watermark all non-Released Drawings with "FOR INFORMATION ONLY" but I keep getting a Relation error on the statement:-


IF PTC_WM_LIFECYCLE_STATE == "RELEASED"
REL_STATUS = " "
ELSE
REL_STATUS = "FOR INFORMATION ONLY"


Anyone got any ideas?


Jase

Put an ENDIF at the bottom of your relations. If you use ProductView for drawings you also need to update the RCP file to regenerate the drawing prior to publishing. This will update the WATERMARK on the drawings to the appropiate verbage.

Here is the one I created for multiple Lifecycle states for reference:


/* BELOW IS THE WATERMARK LOGIC CODE
IF PTC_WM_LIFECYCLE_STATE == "Production Released"
WATERMARK=" "
ELSE
IF PTC_WM_LIFECYCLE_STATE == "Engineering Released"
WATERMARK="THIS DRAWING IS FOR ENGINEERING PROTOTYPES ONLY."
ELSE
IF PTC_WM_LIFECYCLE_STATE == "Obsolete"
WATERMARK="THIS DRAWING AND ASSOCIATED PART ARE OBSOLETE."
ELSE
WATERMARK="THIS DRAWING IS FOR REFERENCE ONLY AND IS NOT AN OFFICIAL RELEASED DRAWING."
ENDIF
ENDIF
ENDIF


Edited by: jsantangelo

 

[Jase]

Thanks James, that seems to have done the trick.

 

[Jase]

This seems to work fine if the Note is applied to a new drawing directly but we are now trying to add this Note directly into the .frm Drawing template so every drawing that is opened and created has this Watermark applied to it.


I am using "WATERMARK" as my parameter on the part, it is part of the startpart.prt file and successfully adds a comment dependant on the "WM_PTC_LIFECYCLE_STATE" parameter to the WATERMARK parameter based upon the Relation below:-


IF PTC_WM_LIFECYCLE_STATE=="RELEASED"
WATERMARK=" "
ELSE
IF PTC_WM_LIFECYCLE_STATE=="OBSOLETE"
WATERMARK="THIS DRAWING & ASSOCIATED PART IS OBSOLETE. DO NOT USE."
ELSE
WATERMARK="THIS DRAWING IS FOR INFORMATION ONLY."
ENDIF
ENDIF


A note has been added to the .frm drawing template stating "&WATERMARK" but when a new drawing is created for the part the note reads "&WATERMARK" regardless of what the "PTC_WM_LIFECYCLE_STATE" parameter says. Any idea's? We assumed the "WATERMARK" attribute would be copied across to the drawing and referencable as per other notes on the .frm template such as "&TITLE_LINE1" or "&CUR_REV" but it doesn;t seem to be. How do we deal with this?


Jase

 

[jsantangelo]

This seems to work fine if the Note is applied to a new drawing directly but we are now trying to add this Note directly into the .frm Drawing template so every drawing that is opened and created has this Watermark applied to it.


I am using "WATERMARK" as my parameter on the part, it is part of the startpart.prt file and successfully adds a comment dependant on the "WM_PTC_LIFECYCLE_STATE" parameter to the WATERMARK parameter based upon the Relation below:-


IF PTC_WM_LIFECYCLE_STATE=="RELEASED"
WATERMARK=" "
ELSE
IF PTC_WM_LIFECYCLE_STATE=="OBSOLETE"
WATERMARK="THIS DRAWING & ASSOCIATED PART IS OBSOLETE. DO NOT USE."
ELSE
WATERMARK="THIS DRAWING IS FOR INFORMATION ONLY."
ENDIF
ENDIF


A note has been added to the .frm drawing template stating "&WATERMARK" but when a new drawing is created for the part the note reads "&WATERMARK" regardless of what the "PTC_WM_LIFECYCLE_STATE" parameter says. Any idea's? We assumed the "WATERMARK" attribute would be copied across to the drawing and referencable as per other notes on the .frm template such as "&TITLE_LINE1" or "&CUR_REV" but it doesn;t seem to be. How do we deal with this?


Jase

If the WATERMARK is in a table in the FORM it will work. If it is a free floating note then you need to use a TEMPLATE for new drawings. This I know from experience when setting it up here. You can also create a user defined symbol that uses the WATERMARK parameter to easily add it to existing drawings.