Windchill and drawing parameters

[SayWhatEh]

Hi, I'm new here, and quite new to Pro/E as well, used solidworks and I-Deas before.


Anyhoop, doing a drawing format for the new company I'm starting at, they are just going to start phasing over to Pro/E.


The drawing form I'm doing uses alot of parameters, and some aretaken from windchill pdmlink. But if I use these parameters in the drawing head (don't really know the english word for that, the place where all the info is written on the drawing), whenever one starts a new drawing Pro/E either asks me to fill in the parameters missing, or just converts the parameter names like "&PTC_WM_REVISION:d" to a text "PTC_WM_REVISION" in the cell. The drawing only gets the PDMlink parameters upon checking in, which is causing me all the troubles. How have you guys solved this problem or am I just missing something?


Oh, the :d suffix for drawing, is that also something you use? I just noticed that it worked since I want to have both model and drawing parameters from windchill on it....


Thanks in advance

/Jocke

 

[vlad1979]

Don't know about "windchill pdmlink" but sounds like you don't have PTC_WM_REVISION parameter created in your models.


All the parameters that you use in your format should be also created in your models. Because when you assign a format to a drawing the format searches for all those parameters in your models. If it doesn't find the parameters it will ask you to create it but it will be created only in your drawing, that's why you see parameter:d


":d" means it's a drawing parameter.

 

[SayWhatEh]

Yeah, Im with you on that. But since the revision info and such for the drawing (not the model) it would be bad to put it on the model. Since the model might have two different drawing linking to it, with different surface finish and other options like that.
Revision information for the drawing I need to have linked to the drawing, and revision info for the model need to be linked to the model.


And anyhow, since I am unable to change how PDMlink saves info, I can't really do it even if I wanted to.


Thanks for the input though... Anyone else?

 

[looslib]

We linked the model parameters to the drawing titleblock. One model, one drawing. Save the model, then the PTC_WM* parameters will be filled in. Since they are driven by PDMLink, they are only generated when the drawing/model is checked in. No way around it.

 

[robertib]

There is a way around this problem - Save & Upload. This puts the files in the workspace on the Windchill server, without putting them into the Commonspace.


The files will have the parameters for version, iteration, etc.

 

[SayWhatEh]

Looslib:
Ah,ok. But there IS a way around it I think, but It's just not totally clear to me yet. For example, if you put repeat regions in the titleblock and set the right filters it will show the parameters, only if there are parameters to show, which will update when you check in into PDMlink.
The issue with this is that I have not found a way to like to drawing parameters yet, only model or assembly. But perhaps you guys now how to access drawing parameters in a repeat region?

robertib:
Save & Upload, you mean the form or the drawing? When in the workflow should I do this to avoid the problems?


Thanks for your input guys!

 

[looslib]

If you want drawing parameters put a :d after the parameter name.

 

[robertib]

Anything you upload to the Windchill side workspace will have the Windchill parameters.


One thing that youwill find usefulto do, is to create a start part (assembly, drawing, format, etc) in Windchill & check into a Commonspace library. Then you can set these start parts to be the ones you create your parts from. These files will then automatically have the Windchill parameters (most of them will be empty, or irrelevant until you unpload, but they will still be available).

 

[SayWhatEh]

robertib, thanks, that sounds like it will solve my problems. Start part, you mean like a template or something? Can one define start parts in the config files?

 

[looslib]

You can define the location and name of the start parts in your config.pro file. There are usually 3 start parts. Detail parts, Assemblies and Sheetmetal parts. You can have more depending on the types of files you create. Start parts are templates that establish parameters, relations, datumns, etc that you want in EVERY file that you create.