5 Replies Latest reply on Jul 18, 2013 2:55 AM by MaBUa

    Symbols from schematic to LibraryManager


      Hello all,

      can somebody help me?

      I have a EE flow 7.9.2 (DxD)

      I have a schematic in which I have a symbols - parts from my library but in Library Manager were some of them deleted . Now I need salvage deleted symbols and put them back to my Library Manager.

      Does somebody know the process to save the symbols?

      (How to export them from schematic.. in which format)


      Many thanks


        • 1. Re: Symbols from schematic to LibraryManager



          I think you are out of luck. I could find no way to save a symbol from DxDesigner and somehow get it in to Library Manager.


          Perhaps now is a good time to have a discussion about data backup. Here's a cautionary tale:


          Early in my career (over 30 years ago) I failed to properly backup a critical PCB project. I was unfamiliar with the data compression utility my boss wanted me to use.


          I ended up creating the compressed file for archiving, but I did not test the file.


          Subsequently, we needed to make a change in time for a trade show. But when I went to retrieve the PCB data I found to my horror that the data was corrupt and unusable.


          With no other backups to revert to we had to redesign the PCB and we missed the trade show. I was put on probation for a month which was just a preliminary before I was fired.


          My first child was born a couple of months before I lost my job, so the lesson really hit home. One learns better from their mistakes than from their successes, and I never lost any CAD data since that time.


          I learned to be very disciplined about backing up data. Every time I exit a project I create a zip file, add to the project name a date and time code and then move it to a network drive.


          What we typically produce in our work is data. Data is everything. Others take our data to make our boards and assemblies, but we produce data.


          Until you are familiar with a particular data backup method, test each backup you make to see if the integrity of the data is still good.


          Do not keep data backups on your computers' hard drive, as you have no recourse should your hard drive fail. Network data is regularly backed up to tape, so keep your data archives there.


          Protect your data. The job you save may be your own!

          • 2. Re: Symbols from schematic to LibraryManager

            Hi Mabua


            Below how you can get the symbols extracted form a schematic so you can import them again in your library.



            How to extract symbols from schematics?


            Since the symbols are cached in DxDesigner project use the following steps to extract symbols from one schematic for use in a new design.

            Export the schematic in EDIF format

            Open a design in DxDesigner

            Use the menu File > Export > EDIF Schematic... to open the EDIF Interfaces dialog box

            In the Schematic/Symbol field enter the schematic name

            Check the Convert Design Hierarchically option

            Check the Map attributes to properties option

            Click the OK button and review the Output results window for any issues

            Import the EDIF schematic into new DxDesigner project

            In DxDesigner create a new project

            Use the menu File > Import > EDIF Schematic to open the EDIF Interfaces dialog box

            In the Inputfield enter the path to EDIF Schematic (.eds) file produced above

            Click the OK button and review the Output results window for any issues

            All of the symbols will be written to the [local symbols] of the new project

            Extract the symbols from schematics

            While still in DxDesigner, select the menu View > DxDataBook to see the created symbols

            Select the CL Viewtab near the bottom of the DxDataBook window

            Next select the Symbol View tab to view the [local symbols] library

            Expand [local symbols] and select all the symbols using the mouse

            Right mouse button on a selected item and choose Export Symbol(s)

            In the Browse For Folder dialog navigate to a location where you want to write the ASCII symbol files

            Click the OK button and confirm that the ASCII symbols have been written


            • 3. Re: Symbols from schematic to LibraryManager

              Is Export EDIF Schematic a licensed option?


              It's not greyed out in the DxD menu, but I receive a license note: No license was found for edifgraphicsmgc.


              No output was generated.

              • 4. Re: Symbols from schematic to LibraryManager

                EDIF export is licensed.

                • 5. Re: Symbols from schematic to LibraryManager



                  many thanks for showing me the possible way to solve it ... it works

                  It's pity there is no possibility to copy the symbol to local lib. inside DxDesigner.... maybe in the future ;-)


                  Bye all