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Drawing frame in part

Tim_1996
7-Bedrock

Drawing frame in part

I have a part model with PMIs and I want to put a drawing frame with model information in there like this:

1.png

I would like to save the model information somewhere like in 2.png and the information should also be exported with a JT or STEP file.

How do I do this?

Thanks!

1 REPLY 1
sacquarone
20-Turquoise
(To:Tim_1996)

Hello @Tim_1996 

 

I can provide guidance in the way to achieve what is shown in attached movie in Part mode.

==> If you're interested in this approach, please keep me posted and I will record a new movie from scratch

 

Before answering, please consider several limitations as follows:

  • The concept need to use custom symbol to achieve this buisness need in Part mode
  • Consider however the limitations officially documented in articles 262908 and  232673, leading in some effort to achieve this:
    1. Produce a cgm file from an image file (the original jpg). Many Free sites proposes this. I personnaly used this one (non PTC applcation).
    2. Table to be built in a drawing (initially empty) where a cgm file was previosuly imported (the new PTC Logo).
    3. Table reformated with merge cells and cgm imported, and converted as "Draft View".
    4. Drawing then exproted as Iges File.
    5. Iges retrieved upon definition process of a new Symbol.
    6. Variable Text definition in Symbol to gather part paralmeters automatically.
    7. Symbol finally placed in the part as shown in the mocie
  • Especially the "images" contained in the table MUST be in Vectorial Format (like CGM), because Raster fortamts (like JPEG, TIFF? etc ...) are not supported

 

Then, once done, please consider we're speaking here about PMI and Combined States. And Combined States :

  • ARE part of definition of parts/assemblies in Creo, and proerly considered also in Creo View (via pvz format) => Check article 286532
  • but ARE NOT part of definition of Step / JT or PDF U3D structures, therefore not supported to be exported in this format => Check article 282931 for the STEP format for instance

 

A backup of material which was used in Creo 8.0 to build attached movie is also attached (second attachment), in case you would like to take an eye on it.

 

Regards,

 

Serge

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