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SM_82849341-Visitor
1-Visitor
October 7, 2022
Solved

Unable to lock/freeze the format just to prevent editing during the drawing preparation.

  • October 7, 2022
  • 4 replies
  • 1951 views
I am using Creo Parametric Release 7.0 and Datecode7.0.2.0

We have our company drawing format where we want to lock/freeze the format [.frm file] just to prevent editing during the drawing preparation.

Here are the errors that I faced
Unable to find any such option to do so
    Best answer by sgudla

    Informed customer that drawing tables present in the format file will be copied over to the drawing during format insertion in to Drawing. This is the intended and designed behavior with tables in a format file.

    If this is NOT needed, Create the Tables using sketch entities and texts. These entities will NOT be copied on to the drawing when format is inserted in to the drawing. As a result, the text contents of these Table looking entities cannot be edited by users.

    4 replies

    H
    hhiller17-Peridot
    17-Peridot
    October 7, 2022

    You cannot protect files by password in Creo Parametric. See https://www.ptc.com/en/support/article/cs93502

    But you can try to use config pro_format_dir for your format files and try to make the directory read only in Windows.

      B
      23-Emerald III
      BenLoosli23-Emerald III
      23-Emerald III
      October 8, 2022

      Formats are copied into your drawing file from either the format itself or by use of a drawing template which has the format in it. Once in the drawing, there is no command in Creo to prevent a user from making changes to the format copy. You can prevent them from saving a modified format by making the format file read-only. There is no way to prevent a user from renaming a format for personal use. This is where ModelCheck can help by checking your drawing files to be sure the formats used are the company standard format names.

      T
      23-Emerald IV
      TomU23-Emerald IV
      23-Emerald IV
      October 11, 2022
      Formats are copied into your drawing file from either the format itself or by use of a drawing template which has the format in it.

      Not exactly.  Tables are copied from the format into the drawing when the format is applied to the drawing, but the format itself remains a separate object that is permanently referenced by the drawing.  Every time the drawing is opened, the format is also opened (behind the scenes). The format needs to remain available and able to be retrieved each time the drawing is opened.

       

      Once in the drawing, there is no command in Creo to prevent a user from making changes to the format copy.

      If the formats are placed in a read-only location (mapped network drive, etc.) as suggested by @hhiller, then users will be unable to save any changes made to those formats back to the location where they are stored and retrieved from.

      TomU_0-1665513244150.png

       

      As you mentioned, this does not prevent a user from doing a 'Save As' on the format and creating their own 'new' copy, but this new version will have to be stored in their working directory or someplace other than the read-only location where all the other formats are being kept. 

      H
      hhiller17-Peridot
      17-Peridot
      October 12, 2022

      This would be an enhancement. You can refer to Product Ideas @ PTC Community and consider posting a new one.

      S
      sgudla18-OpalAnswer
      18-Opal
      October 27, 2022

      Informed customer that drawing tables present in the format file will be copied over to the drawing during format insertion in to Drawing. This is the intended and designed behavior with tables in a format file.

      If this is NOT needed, Create the Tables using sketch entities and texts. These entities will NOT be copied on to the drawing when format is inserted in to the drawing. As a result, the text contents of these Table looking entities cannot be edited by users.

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