5 Replies Latest reply on Jun 7, 2018 2:40 PM by baudot

    Route to a pad

    baudot

      I'm trying to make an ultra-simple break-out board: Every pin on a surface-mount chip goes to a pad on a PCB, so I can solder male headers into the pads for easy prototyping on a solderless breadboard.

       

      The problem is, when I try to route from the chip's pins to the pads, the route dodges the pad! (See attached image.)

      The mouse acquires a symbol, crossed wires, when I try to make the connection. (For reasons unknown, my screen-grab tool doesn't grab it.)

       

      My suspicion is that since the pad was added in the PCB editor, and the schematic is literally just the chip, with no connections, the PCB editor thinks it should indeed be a floating pin, connected to nothing.

       

      How do I get around this? How do I route from a chip to a pad that I've added in the PCB editor window?

        • Re: Route to a pad
          baudot

          Workaround in this case: Remove the pads from the PCB, add headers as a component to the schematic, and wire them together.

           

          Still, what's the point of being able to add pads on the fly in the PCB editor if you can't connect to them? Surely you can, and I'm missing something?

            • Re: Route to a pad
              voltsandjolts

              As you don't have a full schematic that means you probably don't have any nets defined either. You can't connect to the pad because it is not assigned to the net of the track you are editing. You can double click each pad and assign a net for it. You can get the net name from the tracks you create or create all nets in Tools> Netlist > Edit. Probably easier just to create your pad layout as a component and do a proper schematic. 10 mins.

              1 of 1 people found this helpful
            • Re: Route to a pad
              mars01

              I recommend to do what the previous answers said but if you really, really want to do what you proposed to do then go to: File -> System Preferences -> PCB Editor -> Routing Conflict Resolutions -> Current Mode and in the drop-down menu select Ignore obstacles. This will allow you to cross with the track over a pad not in the same net. You'll see the connections marked with a white circle and shortcircuit symbol but it will work if the only thing you want is to do a toner transfer PCB

               

              1 of 1 people found this helpful
                • Re: Route to a pad
                  e14softwareuk

                  To add to this suggestion of using Ignore Obstacles, once you have completed your routing use Tools | Netlist > Configure Physical Nets. This brings up a dialog that lets you turn the copper into actual nets. Gets rid of the short circuit indicators.

                  1 of 1 people found this helpful