The parameter "PTC_WM_Created_by:d" isn't created until the actual drawing for a part is created, preventing it's use in a drawing boarder (for a newly created drawing from a format). How have others tackled this conundrum?
The suggestions I've read are:
Up until recently, our drawings have been part/assembly attribute driven. We're working to correct that, and are driving much more of the content from Windchill. Our template parts now have very little in terms of parameters. This is one of the last hold outs. It seems it's easier to keep it as a parameter.
Have you considered watermarking viewables for drawings instead of pushing any attributes into CAD?
You can do it along with any other parameters you may require (like state, revision, review date, reviewer, etc.).
If you're using a template when creating new drawings, the PTC_*:D parameters will exist when you create the new drawing. However, the values of many of them are not populated until you, at a minimum, upload the new drawing. All the PTC_*:D parameters will have values if you check in the drawing.
If you're using a template, you can create a mapkey to create the new drawing (of the active model), save it, and then upload it (or check it in).
If you're not using a template, you can create a very similar mapkey to create a new drawing. The mapkey would do the following (assuming your model file is the active model):
The problem I've run into (with the former), is that since "PTC_WM_Created_by:d" doesn't exist during drawing creation (from template), is that Creo prompts you for a value for "PTC_WM_Created_by", and once you hit enter? All associativity is lost forever until you replace the template. The field is blank after the prompt upon inital creation, but replacing the format pulls the value because the drawing and associated parameter now exists.
The later certainly works, and it was an option we've been exploring. Creating the mapkeys may make it less annoying and easier to circumvent.
That may work, provided the watermark is retained with the drawing once it's sent to a vendor (outside of windchill). Engineers routine create either pdf's of dwg's for quoting, and we've road mapped some package recipes to streamline the process. For now, they're created from the drawing and saved externally to Windchill.
We don't experience the issue of the PTC_*:D parameters not existing when creating a new drawing from a template, so we're never prompted for any values. I'd suggest you check your template parameters. All the PTC_*:D parameters should exist in your template, and they should be transferred into your new drawing during creation.
Creo Parametric 4.0 M070
Pro/Intralink 11.0 M030
The parameters are there in the template, the value is not assigned until the drawing exists. It's sort of like a circular reference. I've put a parameter in the drawing template title block which references the creator and creation of the drawing. I'd be curious as to how this works with your template part and drawings, or rather, what you are doing differently.
As @dnordin mentioned, the key is to use a template that already contains this parameter. A template is really nothing more than a drawing that is used behind the scenes copy from during drawing creation. The major benefit of a template over a format (or blank drawing) is that the template can contain all of your company's parameters, Windchill's parameters, drawing views, and drawing programs. None of these are included if creating the drawing from a format.
We strongly encourage our users to only create new drawings from templates. If someone makes a mistake and creates a drawing from a format, they will need to manually create the views, run a mapkey to create all the company parameters, run a mapkey to create the drawing program, save the drawing (at least once) to create the Windchill parameters, and then reapply the format to re-sync the title block text back up with the previously missing parameters.
If you're seeing a prompt to enter a value for a Windchill parameter, you're either not creating the drawing from a template, or that template is missing the Windchill parameters. As noted previously, the value of those Windchill parameters will not be correct until the drawing is actually checked in. For this reason, if you're going to print a drawing displaying Windchill parameters, you need to do so after checking the drawing in, erasing from session, and then reloading.
Here's a snip from out title block where we're displaying both the drawing's version and the model's version using these same Windchill parameters:
Oh, I'm sorry. I was confusing formats (*.frm) with drawing templates. I get what you're saying now. My apologies. Yes, we're creating drawing from formats. We used to have dozens of clients with their own start parts, assemblies, and formats (along with drafting standards), and traditionally we would use our client's files over ours.
Things have changed a bit over the past 20 years, and our clients are less interested with adhering to their internal formats and standards, so we can now deliver content on our own formats. Unfortunately, like most overhead efforts, our internal start parts, assemblies, and formats have languished, and we're not capitalizing on our Windchill integration. Our files predate our Windchill integration, so we're still driving border content from parameters.
So, long story short, I've started to revisit our start parts/formats, replacing part/assy level parameters with Windchill attributes. I *thought* I had something that worked - but - my testing method was apparently flawed, as I was using some old drawings to test out some new formats (by replacing the old). The template method makes sense now.
Do you have just a single template per each drawing format? Or are there specific contexts for templates? Meaning, do you have templates for certain types of drawings (machined, sheet metal, assy drawing, etc). Our project vary from medical to defense, and from injection molded parts to machined, so I'm trying to get a feel for the best approach in terms of what templates should exist (or that I should create).
Yes, I do maintain a one-to-one relationship between our formats and our templates. Around 160 drawing templates at the moment. The joys of a CAD admin... 😉