1 Reply Latest reply on Oct 4, 2010 8:57 AM by george_defond

    Mapping one schematic symbol pin to multiple Pads part pins on the same net


      How can I map one ground pin on a DxDesigner symbol to multiple ground pins on a Pads part?  Is this possible?

        • 1. Re: Mapping one schematic symbol pin to multiple Pads part pins on the same net


            I am quoting technote # 50685. Forgive me if it's a little dated, but I have not used dxd in about five years:


          Typically there is a 1-to-1 correspondence between the logical pins on a
          symbol in DxDesigner and the physical pins of a component in the PCB.
          There are however some cases when it is necessary to have a single
          logical pin map to multiple physical pins.  Use the following steps to
          construct the symbol, connect it up, and then to generate the netlist:


               Construct the symbol so that the single (common) pin has a comma
          separated label name for the required pin names - such as A1, A2.
          2.     Add a Pin Number ( # ) property - again, comma separated pin
          numbers to match the pin names - such as 1,2.  This will map pin name A1
          to pin number 1 and pin name A2 to pin number 2.  Make sure that the
          response is NO to the "Expand pins" prompt during this assignment.
          3.     Place the symbol on the schematic and wire a BUS connection to
          the pin.  Make sure the name of the bus has the following syntax
          {NETNAME.EN}#.  In this instance, if the net name was to be FRED the bus
          name would be {FRED.EN}2 - where 2 refers to the connection to pins 1
          and 2.
          4.     After Create PCB Netlist and forward annotating to either
          Expedition PCB or PADS Layout, the net FRED will connect to pin numbers
          1 and 2 of the device used by the symbol.


          Best wishes,


          1 of 1 people found this helpful