Drawings - Fields (e.g. &scale &model_name) not updating

[ptc-267878]

WF4

I have a drawing with multiple sheets. Each sheet has a different part. The master Drawing Format has dynamic fields (e.g. &scale &model_name), but they do not seem to be updating. I change the scale and it is always 1:1, and the model name is always associated with sheet #1. Any suggestions?

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[BenLoosli]

The parameters are only pulled from the first model pulled into your drawing, thus the model and scale of the on sheet 1.
All sheets are using these default values.

In order to do what you want, you will need to build parameters like &scale_1, &scale_2, etc. and &model_name_1, &model_name_2, etc for each model added to each sheet. The information would have to be in a separate table as the format only has the default values in it.

[ptc-1932745]

The sheets can take model parameters, but they do so from the model in session.

If you want different data shown for different models on different sheets, make sure that the required model is in session (by using Layout right click Drawings Models | Select Model (or add model)), and then use 'sheet setup' to re-select the drawing format required. You will be asked to keep or replace the format tables. Select 'replace all' to update the data. This will use the in session model /assembly to fill in the parameters for that sheet.

If you want a particular format to be the same for all sheets (drawing number, for example) you must go to the first sheet and copy the parameter (not the value) from that sheet to the others.

It may have a name like '&drw_no:4'. The ':4' (or whatever) is the important part.

Please note that I am using CE/P 5.0 but the general rules are the same for everything I have used up to CREO1 (I haven't used CREO2 for much yet)


Christopher F. Gosnell

FPD Company
124 Hidden Valley Road
McMurray, PA 15317

[TomU]

The drawing format will display the information from the currently active model at time of creation. If the drawing has the model in it, it will already be in session, but that doesn't automatically mean it's the currently active model on that sheet. With multiple models added to the drawing, just double click on the drawing name at the bottom of the page. A list will pop up letting you choose what model you want to set active. Re-apply the format (as Chris said), and now for that sheet the format will read the information from that model.

Tom U.

[dgschaefer]

Another thing is that if you edit the table cell you'll see something like this:

¶meter:2

The "2" is the session ID for the model that was active when that sheet was created. If you want to change it, you need to find the session ID for the model you want to show and use that instead. You can find the session ID through the relations dialog under Show > Session ID.

If you have a lot of parameters to change, re-applying the format for that sheet with the right model active is easier.

--

[mpeterson]

This is not what you need to correct this or what you want to hear, but more a Fri rant.

I highly recommend ONE part or assembly to ONE detail drawing document.

I know some of the reasons why people and companies want and like multiple sheet drawings with multiple parts, but IMHO I don't think the reasons out way the importance of handling the drawing files and associated models. This question is just another example of how things can get convoluted and difficult such that not all designers and drafters will know how to handle. Develop parts, assemblies, drawing formats and BOM tables utilizing common parameters and KISS.

Mark Peterson
Design Engineer
Varel International
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[ptc-1932745]

Exactly correct. Having a one to one relationship between drawings and parts / assemblies makes things much easier, also make sure that the part name and the drawing name match each other.

Older Engineers at our place used a 'project' paradigm for tooling and fixtures that were used together such as XXX.ASM, XXX-1.PRT, XXX-2.PRT, XXX-3.PRT, etc...all one several sheets of one drawing XXX.DRW

The reasons were twofold, one we did not have any PDM to help find associated parts, and two PTC used to charge extra for Pro/Report on drawings so BOM's were not associative so we did not have this option.

Given the option, I would NEVER suggest having a one-many relationship between parts/assemblies and drawings.

Christopher F. Gosnell

FPD Company
124 Hidden Valley Road
McMurray, PA 15317