DC2DX Migration - DC Library and Project Translation to DxDesigner

Version 11

    DC Library and Project Translation to DxDesigner

    dc2dx3.png

    TOPICS

    Introduction

    Using the DC2DX Virtual Lab

    Translate DCLibrary to DxDesigner

    Translate DC Project to DxDesigner

    Project Synchronization

    DxDataBook Configuration (optional)

     

     

    1. Introduction

    This tutorial walks you through the steps to complete the translation to the Expedition Enterprise flow of a Design Capture Central Library and a Design Capture/DesignView project which is synchronized with an Expedition Layout.  

    This translation process is referred to as “DC2DX”.

     

    Walking through this small tutorial you will:

    • Translate a 2004 Design Capture Library to DxDesigner format
    • [optional] Create a DxDataBook database to use with the translated Central Library
    • Translate 2004 Design Capture Project to an Integrated DxDesigner project
    • Synchronize DxDesigner & Expedition PCB

    The translators used are available on the Expedition Enterprise release media under "Schematic and Layout Translators."

    The DxDesigner Symbol and Schematic Translator User's Guide (Chapter 12 is DC2DX) is available at:

    http://supportnet.mentor.com/docs/201206008/docs/pdfdocs/trans.pdf

     

    2. Using the DC2DX Virtual Lab

    [This section has been removed - the Virtual Lab is no longer active]

     

    3. Translate DCLibrary to DxDesigner

    The first step is to translate the DC/Expedition Central Library to DxDesigner/Expedition format.

    The library translator DCLib2DX uses a configuration file to specify translator settings:

    C:\EE794\7.9.4EE\SDD_HOME\translators\win32\config\dclib2dx.cfg

     

    The configuration file has been set up to work correctly for the virtual lab exercise.  To learn more about the configuation options, refer to the DxDesigner Symbol and Schematic Translator User's Guide (Chapter 12 is DC2DX) at:

    http://supportnet.mentor.com/docs/201206008/docs/pdfdocs/trans.pdf

     

    3.1 Launch DC2Lib2DX Library Translator from Windows Start Menu

    tutorial_3_1.png

     

    3.2 Run DC2Lib2DX Library Translator

    Set up the library translator dialog as follows.

    • Provide a path to the Central Library to be translated:
      C:\Designs\Vidar\Central_Library\Central_Library.lmc
    • Do not check Translate Loose Libraries.
    • Keep the default Config File

    Advanced settings:

    • Do not check Normalize symbols.  This will retain the symbol origins as defined in DC.
    • Check Keep original DC colors.
    • Select Translate.

    tutorial_3_2a.png

    The translator updates the Central Library, creating DxDesigner symbols.  The original DC symbols are retained for reference.

    Upon completion a DCLIB2DX.txt log file is created for review.

     

    3.3 Translating Compound Symbols

    Design Capture symbols can be defined as "compound", where multiple orientations are built into a single symbol.  DxDesigner does not yet support compound symbol definitions in the same manner.  DxDesigner allows the creation of alternate symbols using a numeric extension on the symbol name.  For example, DxDesigner users may create symbols "res.1" and "res.2" to define alternate symbols for horizontal and vertical orientation.   Like Design Capture compound symbols, these alternate symbols contain correct property placement for the symbol orientation.

    tutorial_3_3a.png

    Since DC and DxDesigner symbols work differently, the dclib2dx.cfg config file enables users to choose one symbol or multiple symbols to be translated.

    The configuration file setting is:  CreateRotationalViews=1

    • Setting the value to "1" results in alternate symbols being created, one for each definition in the DC compound symbol.
    • Setting the value to "0" results in just one DxDesigner symbol being created from the first definition in the DC compound symbol.

    The virtual lab exercise uses CreateRotationalViews=1.

     

    3.4 Create a DxDataBook Database

    The translator does not create a DxDataBook database, which many of you may need to use with the DxDesigner/Expedition Central Library.  DxDataBook is not required for the virtual lab exercise, but a database is available in the lab data for those who wish to practice DxDataBook configuration.  Refer to Section 6 of this document to learn how to configure DxDataBook.

     

    4. Translate DC Project to DxDesigner

    With the library translated, we now translate the DC/Expedition project.

    The Design Capture project has been updated to use the power of CES instead of Net Class & Net Properties.  Even if your company does not currently use CES for Design Capture, it is recommended to update the DC design to use CES prior to translation.

    The library translator DCLib2DX uses a configuration file to specify translator settings.

    The project translator DC2DX uses a configuration file to specify translator settings:

    C:\EE794\7.9.4EE\SDD_HOME\translators\win32\config\dc2dx.cfg.


    4.1 Launch DC2DX Project Translator from Windows Start Menu

    tutorial_4_1.png

    4.2 Run DC2DX Project Translator

    Set up the project translator dialog

    • Provide a path to the project file to be translated:
      C:\Designs\Vidar\Vidar.prj
    • User the default Configuration File.

    Schematic Symbols:

    • Select Use libraries which have already been translated.

    Advanced Settings:

    • Check Update time stamps in local libraries.
    • Check Translate CES database
    • Do not check Normalize symbols.  This will retain the symbol origins as defined in DC.
    • Check Normalize designs.  This will set the design origin to the lower left corner.
    • Check Keep original DC colors.
    • Select Translate.

    tutorial_4_2a.png

    After approximately 25 minutes, upon completion a DC2DX.txt log file is created for review.

     

    4.3 Open DxDesigner and Change File Paths

    • Open DxDesigner by double-clicking on C:\Designs\Vidar\Vidar.prj
      The main screen displays the Welcome page.
      The Navigator view displays the project hierarchy.
    • Double-click Vidar sheet 1 to open the top-level Schematic.

    tutorial_4_3.png

    • From the pulldown menu, select Setup > Settings > Project.

    tutorial_4_3a.png

    Observe that the Central Library path is the same as the original Design Capture library path.  The library translator updated the library without moving it.

    tutorial_4_3ba.png

    The Special Components path has been set to an example file from the SampleLib2007 library.  This path must be changed to an appropriate file for this translated library.

    • Update the Special Components path to  ..\speccomp.ini as shown below.

    tutorial_4_3c.png

    4.4 Package the DxDesigner Project

    • Select Tools > Package.  Package in DxDesigner works the same as in Design Capture.

    tutorial_4_4.png

    tutorial_4_4_edit.png

    Package completes with warnings.  In this example the warnings can be ignored.

    • Generate a parts list using the default format by selecting Tools > Parts Lister.

    tutorial_4_4a.png

    At this time the schematic is ready for PCB integration.

    5. Project Synchronization

    Project translation maintains the links to the Expedition PCB design via the project file.  Integrating the schematic with the layout follows much the same process as used in the Design Capture/Expedition flow.

    • From within DxDesigner, select Tools > Expedition.

    tutorial_5_0.png

    Upon opening, Expedition detects that new changes are ready for Forward Annotation.

    • Click Yes to launch Project Integration

    tutorial_5_0a.png

    Choose the flollowing options in the Project Integration menu.

    • Select Delete local data; then rebuild all local data.
    • Do not check Trace removal options - retaining all traces allows manual update which is sometimes required after translation.
    • Select Assign single pin nets to unused pins, enabling fanout, thus being consistent with the setting applied in Design Capture.
    • Click on the amber button to invoke Forward Annotation.

    Once Project Integration is complete all but the Back Annotation lights go green as shown in the picture at right above.

    • Click on the amber Back Annotation light to run.
    • Close the dialog.

     

    5.1 Post-Translation Cleanup

    The original Design Capture/Expedition layout was 100% fully routed layout.  The translated Expedition design displays netlines and reports 86.63% routed, yet all traces exist as previously defined.  This can occur on old (pre-2005) databases due to the loss of plane assignments.

    tutorial_5_1a.png

    • Open the translated design in Expedition.
    • Select Analysis > Review Hazards.
    • Select Online > Open Netlines.  The report indicates that nets "1.25V" and "2.5V" have open connections.

    tutorial_5_1b.png

    Note that all trace connections still exist because in the Project Integration dialog we did not check the option to "remove floating traces and vias".

    • Exit Review Hazards.

    To resolve the problem, re-assign the plane nets.

    • Open Planes > Plane assignments.
    • Add global net 2.5V to Layer 4 and set it to use the route border.
    • Add global net 1.25V to Layer 10 and set it to use the route border.
    • Click OK.

    tutorial_5_1c.png

    • Return to Review Hazards and observe that the board is now 100% routed.

    6. DxDataBook Configuration (optional)

    DxDataBook is not required for the virtual lab exercise.  This optional section describes how to configure DxDataBook using a supplied Microsoft Access database.

     

    Content © Copyright 2012-2014 Mentor Graphics Corp, All rights reserved.

    Product names are trademarks and/or ® registered trademarks of their respective owners.