6 Replies Latest reply on Dec 7, 2010 3:21 PM by MikeD

    Expedition PCB/CES rule

    aaron.palomar

      I would like to create a rule in CES for Expedition PCB that applies directly to text.  In this case text is going to be conductive so I would like to manipulate the clearance from other objects to this conductive text.  Is there a way I can do this?

       

      The problem that I am having with using conductive text is the bounding box for text objects creates clearance errors.  If I could somehow minimize this bounding box by creating a rule it would be helpful.

       

      An example issue: Our librarian has added text objects to Cells in library such as + for polarization markers.

       

      I have experimented with constraints definition but see no way to apply any rule directly to text.

       

      Regards,

      a-

        • 1. Re: Expedition PCB/CES rule
          yu.yanfeng

          There is no direct clearace rule for conductive text to other object, But Expedition will treat conductive text as plane, so it obey clearance rules of plane2trace, plane2via, planetotraces in route mode. However, it doesn't obey any rules when placing conductive text in draw mode.

           

          Yanfeng

          1 of 1 people found this helpful
          • 2. Re: Expedition PCB/CES rule
            aaron.palomar

            Yanfeng,

            Thank you for the input, your response was helpful in understanding how rules get applied to text.

            It would be helpful having the flexability to create a custom constraint where text clearances could be manipulated.

             

            To solve this issue I had librarian change conductive text to conductive shapes. Doing this made area needed for makers much more manageable.

             

            Regards,

            a-

            • 3. Re: Expedition PCB/CES rule
              Jerry_Suiter

              Hello,

               

              Text on conductive layers uses the trace clearances for both Online and Batch DRC.  Therefore Trace to Trace, Trace to Via, Trace to Pad, etc are used where the Text is treated as an Trace object.   Be aware for performance reasons, DRC of text is to the extents box and not to the actual graphics seen as a conductor.  By selecting the text string in Draw you will see the extents box used for DRC purposes.

               

              Also, I would suggest using a Vector Font for text on a conductor layer since it's optimized for stroking and is more accurately seen within the system since TrueType Fonts will require a secondary stroke process during processing for outputs.

               

              Regards,

               

              Jerry Suiter

              Product Marketing Director

              Expedition

              • 4. Re: Expedition PCB/CES rule
                yu.yanfeng

                Hi Jerry,

                I am wrong?  I have veryfied it on 7.9 initial release, it still treats conductive texts as planes and obey plane2trace, plane2via clearance rules.

                Yanfeng

                • 5. Re: Expedition PCB/CES rule
                  Jerry_Suiter

                  Hello,

                   

                  In the end we are both correct since there was an inconsistency between the clearance used for Online versus Batch DRC.  This has been resolved in 7.9.1 so Online DRC is using the Trace-X clearances like Batch DRC does in 7.9 or earlier releases.

                   

                  Regards,

                   

                  Jerry Suiter

                  Product Marketing Director

                  Expedition / Xtreme PCB

                  • 6. Re: Expedition PCB/CES rule
                    MikeD

                    As convenient as it seems, using the plus sign character (+) is not the way to go.  It takes more effort but is much less problematic if you draw two perpendicular lines (hence no text on the Outline layer).