4 Replies Latest reply on Mar 25, 2010 7:04 AM by lsimons

    On/Off Sheet Connector Net Connectivity

    lsimons

      I just found an interesting result of using on/off sheet connectors on a flat schematic over multiple pages.  It seems that on/off sheet connectors are not shorted (linked/connected/etc.) in the netlist (unless the two nets are explicitly set to the same net).  The on/off sheet connectors seem purely aesthetic.

       

      I was wondering if someone could verify this is the normal behavior of DxDesign?

       

      Thanks,

      Louis

        • 1. Re: On/Off Sheet Connector Net Connectivity
          atannen

          It's interesting that you should mention the problem with DXDESIGNER.  I use ORDAD Capture for Schematic capture and I have noticed that the Voltage connections don't necessarily connect from page to page even though I'm using a "VCC Bar" or "VCC Circle" to reference it.  It will not make a proper connection unless I specifically use at least one off-page connection.  I don't know why this happens, but in this case, that was the solution.  I hope that this is, in some way helpful to you.

           

          Andy

          • 2. Re: On/Off Sheet Connector Net Connectivity
            lsimons

            Hi Andy,

             

            It sounds like Orcad is behaving (almost) as expected.  There is probably somewhere to specify global nets (and the vbar/vcircle) don't happen to be included by default.  By using an offsheet connector, Orcad knows to short the vbar/vcircle across sheets.  I haven't used Orcad enough to really know what's going on.  Hopefully someone will chime in.

             

            Unfortunately, by default, DxD seems to not apply any logic to cross-sheet connector symbols unlike Orcad.

            • 3. Re: On/Off Sheet Connector Net Connectivity
              robert_davies

              On/Off Sheet connectors are only used for annotation (cross referencing) and do not drive the connectivity, this is driven by net name association. It is possible to have different net 'names' to on/off sheet connector 'names' and the connector name is ignored by the net lister. Port names, those that drive connectivity between hierarchical blocks and the child schematic are driven the Port Connector symbol name, which is a 'PINTYPE' component in DxDesigner as opposed to an 'ANNOTATE' type for the On/Off sheet connectors. In the case of Port connectors the name of the connector directly links with the pin of the parent block. In this case the use of a different net name is supported and the resultant 'flettened' net will be that of the net at the top of the hierarchy.

              Global nets are driven by special 'TAP' symbols with a NETNAME property which corresponds to the global net name. Being global they do not need to be propagated down through the hierarchy but wherever you want them connected to a component pin a net stub must be connected to the pin and terminated by an appropriate 'TAP'.

              See this discussion http://communities.mentor.com/message/10641#10641

              • 4. Re: On/Off Sheet Connector Net Connectivity
                lsimons

                Hi Robert,

                 

                Thanks for the feedback.  I didn't realize they were only graphical annotations.

                 

                Regards,

                Louis