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byork17-Peridot
17-Peridot
July 17, 2013
Question

Using PTC_WM_REVISION:D in a drawing format

  • July 17, 2013
  • 9 replies
  • 4651 views

If I usePTC_WM_REVISION:D in a format it will not work on new drawing that have not yet been saved. It will prompt for the value because it doesn't yet have the parameter in the drawing until it is saved. I know I can use a template as a work around for new drawings but is there a better way that anyone has found? I would prefer not to have to reapply the format either.



Thanks in advance!


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9 replies

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TomU23-Emerald IV
23-Emerald IV
July 17, 2013
This whole thing is a big mess. Windchill and Creo/Pro are NOT integrated in this area. After a very extensive tech support case it basically came down to, "file an enhancement request". The case details are attached as a PDF if you're interested in reading them. And no, I have not created an "idea" in the community yet. I would have to figure out how to concisely summarize all the related issues first.

Tom U.
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AndyHermanson14-Alexandrite
14-Alexandrite
July 17, 2013
Tom what version was this in? I was able to do this in Creo Parametric 2 M020 I believe. I have a table in the drawing that calls the rev for the model and rev of the drawing as well as lifecycle states.

Andy Hermanson
Engineering Design Applications

tel 605.275.1040 x51114 mobile 605.951.0168
website www.daktronics.com
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TomU23-Emerald IV
23-Emerald IV
July 17, 2013
This was actually in WF5 M120 (CE/Pro 5.0), but I did test it in Creo Parametric 2.0 M020 and had the same results.

You CAN create a table and apply it to a drawing. You CAN create a format with the table in it. You CANNOT create a template that will maintain the correct information unless you reapply the format (with related table) after the drawing has been created. You also cannot successfully create a new drawing (with the table parameters correct) by referencing only the format. Since the parameters do not yet exist in the drawing they automatically snap to the model instead. Again, the format has to be reapplied after the drawing has been created. This whole mess gets even more complicated for drawing programs (in templates).

Tom U.
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davehaigh13-Aquamarine
13-Aquamarine
July 17, 2013
The issue here, comes down to one issue, the fact that you can’t pre-designate parameters in a drawing template.
This has been a major gripe of mine for a long time.

We do our templates like this:

· Outside of template mode, we create the drawing program. The drawing has no parameters. It gets them all from the program. The model added to the drawing before creating the program has no parameters either. The model is removed from the drawing before switching to template mode.

· Inside of template mode, we add repeat region tables, formats, views, & standard notes.

Go to my ProE Admin 101 talk and download the drawing_program.zip file. That contains an .avi movie of how to do a drawing program.
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BrentDrysdale12-Amethyst
12-Amethyst
July 17, 2013
Hi Folks,
Not sure if it is in any way relevant as we don't (yet) use Windchill.

However the parameters thing in drawings is something I worked around by
having only calling parameters and notes from the model itself. Thus when
making a drawing for a part or assembly the Drawing template Title Block
auto populates from the information in the model. The Template part and
assembly have default values for all notes and parameters otherwise it does
not work. The user can update the model information before or after making
the drawing and from a checking point of view it is very easy to see if a
drawing has default information and therefore that the model needs to be
updated. It coincided nicely with my model-centric approach anyway. Has
worked robustly for nearly five years now.


Regards,

*Brent Drysdale*
*Senior Design Engineer*
Tait Communications
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BenLoosli23-Emerald III
23-Emerald III
July 18, 2013
It all works fine IF you use model parameters in your drawing formats. The issue is using drawing parameters in your format. Then you have issues becasue the parameters don't exist before the drawing is saved in Windchill. Even if using model parameters you MUST save the model file before creating the drawing or the you have the same issue of the parameters don't exist yet.

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AndyHermanson14-Alexandrite
14-Alexandrite
July 18, 2013
So this is where ours probably differ. We don’t actually switch them to template mode. We save the drawings in a directory and pull them in on new drawing creation.

Andy Hermanson
Engineering Design Applications

tel 605.275.1040 x51114 mobile 605.951.0168
website www.daktronics.com
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davehaigh13-Aquamarine
13-Aquamarine
July 18, 2013
Ok, I grant you we are not using drawing parameters, all the parameters in the drawing are driven by the drawing program, so they equal the model parameters.

However, our start parts have all the parameters in them already. I don't experience the requirement to save the model before creating the drawing using the template.

Also, Because I have a number of users with laptops, we don't look inside windchill for the start parts and drawing templates. Those files are archived in Windchill, but they are copied to a network share folder so they can be accessed normally. This allows making those files/folders available offline, so that when the user has their laptop at a remote location, they still have access to all the config files and start parts, etc.

David Haigh
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BrentDrysdale12-Amethyst
12-Amethyst
July 18, 2013
Hi Folks,
Just in answer to Ben's point this is why our template parts and assemblies
have all parameters and notes filled in with default values. As has been
pointed out if the drawing "sees" something missing it stops and asks for
it and to the best of my knowledge it has always been this way for ProE.
As soon as this happens any associativity is lost and I was looking for
bulletproof. The risk in the system we use is that the defaults do not get
changed but this is obvious in any drawing and it could be checked for in
ModelCheck or possibly in Windchill but I an not familiar with either
process.

I think in a model centric way and to me drawings are just some of the way
we convey information. For many of our parts it is not even possible to
fully dimension them so it keeps coming back to the model.
I know that for some places drawings are king and they put a lot of
emphasis there. Can't help for that side of things 🙂


Regards,

*Brent Drysdale*
*Senior Design Engineer*
Tait Communications
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