1 Reply Latest reply on Nov 26, 2009 1:56 PM by robert_davies

    Defining border attributes and border.ini file location

    SHWTIME7

      We have schematic sheet borders that were translated from the DA LMS world to DxDesigner. The only problem is we are not able to modify the attributes that carried over. Everything is locked out unless you are in the border symbol itself and that is not where we want to update information. Even to create a new one is a bit cryptic to me. Especially since I was a Design Capture guy for so many years.

       

      Once the border is placed you can not select anything. Also, Is there a detailed explanation on how to setup the attributes required in the borders symbol so that we can select and edit them accordingly in DxDesigner?

       

      I am looking for an example borders.ini file that I can use as a template or a better explanantion (than Mentor) on how to build the .ini file so that we can update the border, be it a constant or auto-generated attribute doesn't really matter.

      We are looking for some examples or clarification to setting one up and actually get it to work when updating the border in Dx.
      Also, I am defining the location for the borders.ini file to be located in the Central Library and I want to add it to the DxDesigner environment so that when a new project is created by the EE it will automatically read the corporate borders.ini file. Now, how can I setup everyone to see that .ini file via their WDIR directory? Is there an environment variable?
      Any insight or feedback would be greatly appreciated.
      It was so much easier to work with these issues in Design Capture.
        • 1. Re: Defining border attributes and border.ini file location
          robert_davies

          Setting up border data in DxDesigner is not that much different to Design Capture, but there are a number of things you need to consider. Firstly the border data itself is driven from the Border Symbol, much as in DC. You may add the information you require to appear in the border as Properties (placeholders) on the sheet border symbols. Add any company specific properties to the Property File (prp) file first, then place them on the sheet border symbol. We provide a number of auto-generated types (different mechanism to DC), they are available in the symbol editor when you edit the symbol, they all have @ as the first character. You will not see these in the Property File, they are managed as special internal properties; available auto-generate properties are @SHEET, @SHEETTOTAL, @NAME, @DATETIME, @PATH.

           

          If you look in the SampleLib provided in the install tree there are a couple of example Sheet Borders with properties applied, the A1 Border for example has the @ properties plus AUTHOR and REVISION. The latter two need to be added to the prp file to be used.

           

          Once the properties are on the border symbols they can be updated via the DxDesigner schematic editor. It is the editing of the data that actually creates or updates the borders.ini file, the file is used to make the data persistant.

          The data (apart from the @ properties) are edited via the Setup - Settings dialog. Look in Setup - Settings and under the Designs section you will see the Borders sub-section. This is where you associate the border symbols used with each sheet size. There is also a button here labelled 'Properties' if you select this it will open an edit dialog listing the Properties associated with the sheet border, this is where you update your values, in the A1 example AUTHOR and REVISION would be listed.

          After doing your edits and closing this dialog you must update the data in the schematic from Edit - Update Properties. This provides you with scope options, Project, Design, Schematic and Sheet, these options support the concurrent use model of the database and allow you to update sheets from the current opened sheet to the entire design or project (the project may have more than one design (PCB) associated with it). The auto-generated properties will be updated at the same time.

          This data is written to the borders.ini file for the project, you will see this if you open the borders.ini file in a text editor.

           

          You also mentioned two other issues with the Sheet Borders which I will cover here. Selection of the Sheet Border symbol in DxDesigner and creating a Borders.ini file.

          Selection of the sheet border is done by setting it as selectable in the Selection Filter and then selecting an area in the bottom left of the symbol. As you say it is a bit cryptic so I will explain some of the mysteries here. The border symbol is what is known as an Annotate type symbol so does not get passed to PCB layout, but like all symbols in DxDesigner it has a 'bounding box' used by the Avoidance Routing mode of the schematic editor. The cursor cannot be placed inside the bounding box when using avoidance mode other than for selection of the object. In general the bounding box extends to the outside edge of all symbols up to and including the pin boundary. Now for a Sheet Border having a bounding box extending to the edge of the symbol will prevent you selecting anything inside the symbol, you would not be able to place components or draw nets on the sheet if we did this. So for Sheet Borders we draw a very small bounding box ( 0.1 x 0.1 inches) near the symbol origin (usually the bottom left). This is the reason you have to select the Sheet Border at this point.

           

          Finally creating a Template Project. This may not seem related to the second issue but it is.

          In DxDesigner you can create template projects that you re-use to seed new designs, the template project may include the Central Library pointer, special components settings, border settings etc. In fact almost any persistant setting you wish to predefine. In the case of the borders.ini file and speccomps.ini file this is the process you need to use to set them up.

           

          In DxDesigner create a new project (File - New Project) and under the Project node of the Setup - Settings dialog define the pointer to the Central Library (you may use environment variables for this, declare them using  ${ENV_VAR} in the string) and configure the special components file and the borders.ini file to be local to the project ( .\speccomps.ini and .\borders.ini). Then under Special Components add your power, ground and onsheet/offsheet and port connectors and in the Borders settings define which Sheet symbol is associated with each sheet size you use.

          If these are all the settings you want to configure exit DxDesigner.
          Browse to the folder where you created this new project and you should see a *.prj file and the speccomps.ini and borders.ini files you have just created. Copy all three of these files to the templates area located in your user WDIR directory: $WDIR\Templates\DxDesigner\Expedition (you can do the same for the Netlist flow).

          Start DxDesigner and create a new project from File - New Project. In the New Project dialog you will see your template project listed under the Project Templates Node. Use this to seed your new project. The Central Library pointer will be automatically configured and because you set the special components and borders files to be local to the project in the template the speccomps.ini and borders.ini files will be copied from the templates directory to the new project's directory and will be configured as in the template project.

           

          If you have any further questions regarding this email me at robert_davies@mentor.com

          3 of 3 people found this helpful