3 Replies Latest reply on Apr 16, 2015 3:16 AM by y.hubert

    Annotating schematic

    jernej

      Hi everyone!

       

      I am new and trying to learn to use PADS(DxDesigner).

      I somehow managed to figure out how to create schematic, how to create libraries and how to route PCB(all steps seperately, not together as I will explain).
      I am having problems with annotating the schematic.

      For a starter, I put few resistors(copied form Optimum Design Libraries), few capacitors(same as resistors) and few ICs(my design) into schematic.

      Resistors have reference designators "R?", capacitors "C?" and ICs "U?".

      But when I run the packager, it replaces all Ref Designators with Un (n is a sequence number of the element, basically, all Rs and Cs are replaced with Us)!

       

      Somehow, I could not find the settings to correct this!

      Also, I am wondering, why can't I replace existing reference designator (for example: U2) with default "U?". The question mark is reported as being invalid option.

      But when designing a library, it is perfectly valid to use "U?" for reference designator.

      Why so?

      Am I missing something?

       

       

      regards, Jernej

        • 1. Re: Annotating schematic
          robert_davies

          The prefix followed by the ? defines the valid values for a reference designator, by convention this is Un for an Integrated Circuit and Rn, Cn, CRn for resistors, capacitors and diodes (based on US conventions) where n is a number that is incremented by the net lister to make them unique. If you want to use something else you can define this in the symbol editor, say IC for an integrated circuit, so you would add IC? to the symbol.

          There are two configuration files that control the 'legal' set of characters you may use, one is the *.cfg file used by the netlister to create the output files for PADS layout, the other is the 'Property definition file' used to verify characters on-the-fly as you type them into the 'Properties' dialog. The issue you have with not being able to set the value back to U? is because the property definition file is not allowing this. You can edit this file from Tools - Property Definition Editor - best practice is to copy the one from the installation directory into a location defined by your WDIR path, and the recommendation is to have three paths: Your local writable one where your personal changes get saved, a 'shared' location which all users can get to (if you work with more than one engineer and share the tools) and the installation folder. The new netlist.prp file should be copied to the intermediate file location and referenced in your project from the Settings dialog (see picture). If you edit the REFDES property to include the ? as a legal character you will be able to add U? or R? as a value in the 'Properties' dialog (see second picture).

          If your symbol definition includes the U? on the symbol then rather than attempting to type this into the 'Properties' dialog simply select the property in the dialog and with the right mouse button context menu select 'Delete Property' this will set it back to the symbol level definition of U?.

          For the second issue, though it is not clear it looks like you are saying all resistors and capacitors that have R? or C? are getting a Un value as well. If this is the case then the *.cfg file you are using will need to be modified, please review the on-line help on this one or open a call with your support representative as this is not my area of expertise.

          • 2. Re: Annotating schematic
            song.lin

            "Resistors have reference designators "R?", capacitors "C?" and ICs "U?". But when I run the packager, it replaces all Ref Designators with Un (n is a sequence number of the element, basically, all Rs and Cs are replaced with Us)!"

             

            I am having similar issue, with all resistors' designators changed to Un after packaging. Would anyone please suggest how to fix it?

            • 3. Re: Annotating schematic
              y.hubert

              Hi,

               

              When you create the "Part" asociated to teh Symbol, in the "General" tab, be sure the "Logic Familly Reference Prefix" is correctly defined.

               

              If you leave it as "Undefined", you'll see when packaging that the Reference designator defined in the Symbol file is replaced by Ux.