Format issues (&PTC_WM_REVISION:D)

[Patriot_1776]

We have older formats that use the old Intralink parameter (&PROI_REVISION:D) that works just fine when you create a new dwg that's never been in Windburn, er, Windchill. I just updated our formats with a new corporate logo and updated the revision parameter to the Windchill rev parameter (&PTC_WM_REVISION:D) and the performance is buggy. When replacing the old format with the new format, it works fine. When creating a new dwg, the revision parameter string drops the "&", and sometimes the ":D" as well, and will no longer work. I double-checked our new and old .frm (format) files, and they're what should be correct, ("&" prefix and ":D" suffix), yet the old format works fine, and the new one doesn't. Is this glitch simply a Windchill thing? Are we going to have to deal with this every new dwg we make? Should I just use the old parameter because it actually still works?

WAAAY annoying.....

Any ideas?

Thanks!

[dschenken]

I think that dropping the & occurs when there is no matching parameter available. Perhaps if the drawing is saved before the format is added the drawing will get the Windchill parameters assigned and be ready to use.

[Patriot_1776]

Interesting. I'll have to try that! Do you mean "saved locally", or "saved in Windburn"?

Thanks!

[Patriot_1776]

Ok, the steps my co-worker took was to create a new drawing, with format, then saved it, which worked with our old formats (Intralink revision) but is not working with out windburn revision.

[Patriot_1776 · Accepted solution]

Well, one issue I found is that the parameter &PTC_WM_REVISION:D" (all parameters) are not created until you save, so if you create the dwg with a format, it does not/cannot creat the parameter, so the string in the format gets truncated and does not work, becoming just the text string "PTC_WM_REVISION".

Whatever the best fix turns out to be, however, I have a fix:

Ctreate the dwg without the format ("Empty" option), then save it, THEN add the format. The act of saving itself creates the needed parameters, and then the format works just fine.

We'll be doing this until I can figure out why the Intralink parameter works, but not the Windchill one.

[llie]

Frank,

I just went through and updated all of our formats to reflect the correct PDMLink attributes and discovered the same thing.

"Create the dwg without the format ("Empty" option), save it, then add the format.

The act of saving it, creates the needed parameters, and then the format works just fine."

We are developing a toolkits to create drawings that will bypass this agony.

[Patriot_1776]

Well, I hope my Pro/WINDCHILL-WORKAROUND helps you or others. It seems to work for me. A little annoying, but only a few easy/fast extra steps. One day I'll find the root of the issue.

[TomD.inPDX]

If you're not careful, Frank, PTC will make Pro|WorkAround an optional extension!

I can see a business case where this can really boost the bottom line

Obviously this should be reported to the Windchill support team. Something is seriously out of sync.

[Patriot_1776]

....I've already got the patent on the Pro/FANITY module!

[ryankelley]

You guys are too much...

Antonius does make a good point, if this is a particular pain point for you, you should absolutely log a case with the Windchill support team and provide them with the workaround.

[Patriot_1776]

Ok, that's a good suggestion, and when I'm not so busy I will, but.....now I'm solving PTC's problems, for free?

[llie]

Aren't we all solving PTC's problems or finding work arounds?

[TomD.inPDX]

I have actually found that posting unlisted YouTube videos works very well with support.

They have the full issue and they can work on it without having me walk them through it again and again.

Even a CamStudio capture will resolve to HD on YouTube.

[Patriot_1776]

Bwahahaha!

[JoshuaHouser]

I hate to stir the kettle again (not really), but is everybody still using work-arounds to update the PTC_WM_Revision parameter on new drawings?  I checked the new system, but could not find an enhancement request/idea/lightbulb, etc.

[TomU]

This is a pretty old thread.  There are definitely newer ones out there on this topic.  I guess the question is, are you trying to show the revision of the model or of the drawing?  If drawing, then the only option is

:D (&PTC_WM_REVISION:D)

This will fail (turn into dumb text) if applied to a drawing before the parameter exists (basically anytime you create a new drawing from a format).  On the other hand, if you are trying to show the revision of the model you can either use the 

:MDL syntax (&PTC_WM_REVISION:MDL)

or a single cell repeat region.  The :MDL syntax does not resolve until a model is added to the drawing, so it won't fail if creating a new drawing from format, but it will fail if removing the model from the drawing.  The single cell repeat region is very robust and won't fail no matter how the drawing is created.  Once the parameter is available, it will properly evaluate.

(&MDL.PARAM.VALUE with repeat region filter set to &mdl.param.name  == PTC_WM_REVISION)

[JoshuaHouser]

Thanks @TomU.  Yep, an old thread...I searched for a more relevant thread and couldn't find anything addressing the issue as well as this.  I'm trying to get used to the new forum (and wondering which of my profiles this one uses).

Anyway, I see the "mdl" extension points to the model and not the drawing.  This is a change to our data model and will likely not be acceptable

(we use @PTC_WM_REVISION:D)

[cschmid]

Has anyone found a newer solution to this issue? This is bugging the hell out of my engineers along with many other PTC quarks new to CREO. 
Can someone help me with a solution besides opening as empty saving then changing format?

[BenLoosli]

Are you using formats for your initial drawing creation or templates?

By using a template file, you can create the drawing and not lose the &wm_ptc_revision:D string in the new drawing, even if the drawing has not been checked in. When you do check in the drawing, the format table fields will update to shoe the drawing revision.

The templates we use are the formats with some additional symbols added. The symbols have to be at the template level as they also have parameters that get populated after the designer has updated the parameter fields.

[Patriot_1776]

Honestly, it's not a big deal once you know the fix, dunno why they're whining.  Are they former SolidQuirks users?  If so, that explains the whining in general.....  😉