7 Replies Latest reply on Jun 22, 2011 3:49 PM by David Ricketts

    Connecting different GND planes together?

    Pete

      I thought I had seen something about this in release notes somewhere, but I can't find it now.

       

      I have multiple GND planes (digital, analog, RF, shield) that all need to be referenced together at a few locations on the board.  I've got some tricks, like copper only decals with overlapping pads.  But to use these with an IPC netlist test in my CAM editor, I have disconnect them all, run the artworks and checks, then reconnect them to run final artwork.  I don't like having to cheat software to get what I need.

       

      Is there some function in PADs to connect two different nets?   Does anyone have other ways of doing this?

       

      Pete

        • 1. Re: Connecting different GND planes together?
          yan_killy

          Hello Peter,

           

          Couple releases back we have introduced a special type of Copper for shorting two or more electrical nets. Electrically of the schematic they are still have it's own identity like GND, AGND, PGND, etc.

           

          Once you add the piece of Copper and got into Properties to add the Net it will belong, you will see a newer feature called Bridge. Once you select Bridge, you will be able to assign to that copper multiple net names.

           

          Benefit of this is that Clearance Check will not flag you with an error and Connectivity will see individual Nets not shorted.

           

          Regards, Yan

           

          Bridge.jpg

          • 2. Re: Connecting different GND planes together?
            jduquette

            Peter,

             

            Long before PADS introduced the 'bridge' method I developed a 'jumper' component that is a short on the board with two independent nets on either pad.  I like it better because it does show the connectivity on the schematic.  While it does cause clearance errors, these are easy to filter through because all of my 'by design' clearance errors will be on components with "JU#" reference designators.  I archive a 'clear.lst' report when I release a design, so that I can verify I don't have additional errors when a layout is revised.

             

            If you are interested in this approach I'll post my jumper component and decal.

            • 3. Re: Connecting different GND planes together?
              RLS2004

              I like to see how other designers handle problems. I'd like to have a look at your jumper component/decal solution to this one if you'll post it!

              ... RLS

              • 4. Re: Connecting different GND planes together?
                jduquette

                I believe this is everything you need to import this part into your library.  This is a jumper with pads matching an 0805 component.  If I need to separarate the traces I can cut the trace in between and install an 0805 for whatever impedance I need.

                 

                In my clearance report I'll see this:

                 

                ----------------------------------------------------

                Error   1 Location 1374.23,2136.62 Level 1

                Distance between pads too small:

                JU7.1, JU7.2 overlapping

                 

                 

                As long as I see the pads are on a component with a JU ref des I know it is a non error.

                 

                Comments and questions welcome.

                • 5. Re: Connecting different GND planes together?
                  wolferm

                  I have also done the same thing with (back in the day) Cadnetix, thru Dazix thru VeriBest to Expedition, and on Altium also probably same method as jwheeler.

                  I just made a few of them to match trace width I was connecting with.

                  But all you are really doing is creating a decal that is made up of two overlapping pads. Yes you will get

                  and error but they are easy to see & move on to real errors. I made a few of them so that the pad sizes were exact same width as

                  the trace I was connecting together, say 10mil, 15mil, 25mil, 50mil wide, then length as short as possible or needed.

                  That way when done within a trace you see the ref des but other than that it looks like it is just a contiguous trace only.

                  In tying two plane areas together you could still use the same thing, using it as the bridge trace between planes.

                  If you didn't want these pads as exposed copper you have to remember to set soldermask pads to 0 or - the size of pad pending cad system used.

                  Bob

                  • 6. Re: Connecting different GND planes together?
                    Pete

                    Thanks to all!

                     

                    Bridging copper was what I was trying to remember.

                     

                    I do also use components to do this on the board, to allow it to be shown on the schematic.  In this case, we were trying to emulate what we had done with copper tape, without showing it on the schematic, so the bridged copper did the trick.

                     

                    One thing I had hoped would be different with bridged copper was the IPC-356 netlist.  I have to open all of the shorts, whether made through overlapping pads or bridges, to run artworks for an IPC-356 netlist comparison in my gerber editor.  Kind of risky to run the check, then go back to the version with all fo teh shorts closed.

                    • 7. Re: Connecting different GND planes together?
                      David Ricketts

                      I was concerned about this too, but with 9.3, and possibly earlier, I didn't check, the PADS generated IPC netlist is correctly amended to report the copper bridged nets as a single re-named net.