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sloman1-Visitor
1-Visitor
March 21, 2013
Solved

Create part name in a note

  • March 21, 2013
  • 5 replies
  • 8663 views

How can I get the part name in a note? I have tried &model_name, but then the name of the assembly is displayed.

Knipsel.PNG


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    Best answer by dgschaefer

    Another way to do this is to find the part's session id.

    Open the relations dialog (Tools tab > relations) and then pick Show > Session ID, pick Park in the pop up menu and then pick the part in question on screen. The session ID will be shown in the message area. Then create a note with this text '&model_name:ID where ID is the number you just found.

    Another method would be to create a user parameter in your part tied to the file name. Enter the relation file_name = rel_model_name in the part's relation and then use &file_name:att in your note attached to the model.

    5 replies

    D
    dgschaefer21-Topaz II
    21-Topaz II
    March 21, 2013

    If your note is attached to the edge of the model in question (and not an edge created by a section, for example), you shoudl be abel to use &model_name:att).

    Dale_Rosema
    23-Emerald III
    Dale_Rosema23-Emerald III
    23-Emerald III
    March 21, 2013

    Doug,

    Is the ":att" the number of the model in the assembly? How do you find that number?

    Thanks, Dale

    D
    dgschaefer21-Topaz IIAnswer
    21-Topaz II
    March 21, 2013

    Another way to do this is to find the part's session id.

    Open the relations dialog (Tools tab > relations) and then pick Show > Session ID, pick Park in the pop up menu and then pick the part in question on screen. The session ID will be shown in the message area. Then create a note with this text '&model_name:ID where ID is the number you just found.

    Another method would be to create a user parameter in your part tied to the file name. Enter the relation file_name = rel_model_name in the part's relation and then use &file_name:att in your note attached to the model.

      S
      sloman1-VisitorAuthor
      1-Visitor
      March 21, 2013

      Doug!

      It works, thank you!

      Knipsel.PNG

      Dale_Rosema
      23-Emerald III
      Dale_Rosema23-Emerald III
      23-Emerald III
      March 21, 2013

      What method did you use - the ID?

      V
      VladimirPalffy14-Alexandrite
      14-Alexandrite
      March 21, 2013

      Hi,

      ...if I need to check the corect information "att_mdl" for note in drawing - I create "fake relation" in assembly mode - system automatically create for me information (behind parameter in relation) and then I can use this number to my note in drawing

      For example:

      note.JPG

      S
      sloman1-VisitorAuthor
      1-Visitor
      March 21, 2013

      Now I have made a "mapkey" to search for the session ID. In the mapkey is also the command for making the note. It takes seconds to place the part numbers in a assembly.

        V
        VladimirPalffy14-Alexandrite
        14-Alexandrite
        March 21, 2013

        I like mapkeys too -

        Here is some Trisks with Mapkeys and video Hide custom Layers with Mapkeys

        V
        VladimirPalffy14-Alexandrite
        14-Alexandrite
        March 22, 2013

        I have created idea for new release

        What do you think? Vote here: Enable Show/Hide Session ID in Model Tree

        C
        ClearBlueSky851-Visitor
        1-Visitor
        February 2, 2015

        For some reason I have found that I have to enter the parameter in lowercase &model_name and uppercase &MODEL_NAME does not work. For multi-part drawings, whatever model I have active, ProE / Creo will append the correct number at the end e.g. &model_name:12

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