4 Replies Latest reply on Sep 5, 2017 2:56 PM by wilykat

    mystery air wire in my project

    wilykat

      https://www.dropbox.com/s/p0y0s7xhj8qqhb7/LED%20cube%20board.brd?dl=0 my current WIP at this point.

       

      Can anyone explain the air wire between GND and VCC near the bottom?  Picture: https://imgur.com/on0AMd8 the pink arrow.  There's also a few yellow X's where the trace connects with decoupling capacitor pins, like Eagle doesn't know those traces are connected with capacitor's leg.

       

      I don't have the schematic for this one, I got the original one from https://www.oshpark.com/shared_projects/LyWFDL0A   There was some mistakes with the original board, some grounds rails weren't connected, and the decoupling capacitor was in series between VCC rail and the chip's VCC pin, this would have isolated and prevented all 9 chips from getting power. I changed the caps so all VCC pins were connected directly to VCC rail, and the capacitor now connects from VCC to ground. Also fixed a couple missing ground connections to the 16 transistors and to ground pin of one of the chip.  It's almost like the previous person designed the board without using Eagle's schematic for some reason?  Oh and I added text of pin function with the 2 pin headers, marked all 9 chips, and noted all resistor (except one marked 330) and all capacitors are the same value 100 and 0.1uF

       

      Anyway can someone double check that I don't have VCC and ground crossed and see why there's air wire trying to connect that 2?  It'd be around $60 down the drain if the board was useless because I missed something.

       

      Still to do: replace 16 pin header with 12 as 4 of the pins aren't used and one pin (15) is in the way of the circuit trace.

        • Re: mystery air wire in my project
          CadSoft Guest

          On 05.09.2017 11:16, Eric Chapin wrote:

          https://www.dropbox.com/s/p0y0s7xhj8qqhb7/LED%20cube%20board.brd?dl=0 my current WIP at this point.

           

          Can anyone explain the air wire between GND and VCC near the bottom?  Picture: https://imgur.com/on0AMd8 the pink arrow.  There's also a few yellow X's where the trace connects with decoupling capacitor pins, like Eagle doesn't know those traces are connected with capacitor's leg.

           

          I don't have the schematic for this one, I got the original one from https://www.oshpark.com/shared_projects/LyWFDL0A   There was some mistakes with the original board, some grounds rails weren't connected, and the decoupling capacitor was in series between VCC rail and the chip's VCC pin, this would have isolated and prevented all 9 chips from getting power. I changed the caps so all VCC pins were connected directly to VCC rail, and the capacitor now connects from VCC to ground. Also fixed a couple missing ground connections to the 16 transistors and to ground pin of one of the chip.  It's almost like the previous person designed the board without using Eagle's schematic for some reason?  Oh and I added text of pin function with the 2 pin headers, marked all 9 chips, and noted all resistor (except one marked 330) and all capacitors are the same value 100 and 0.1uF

           

          Anyway can someone double check that I don't have VCC and ground crossed and see why there's air wire trying to connect that 2?  It'd be around $60 down the drain if the board was useless because I missed something.

           

          Still to do: replace 16 pin header with 12 as 4 of the pins aren't used and one pin (15) is in the way of the circuit trace.

           

          The VIA there is logically connected to that blue net, and I think it is

          not connected to the overlapping. Yellow cross means there is an

          vertical airwire between layers.

           

          Use show on the nets or vias and you will see the whole net highlighted,

          and maybe find connections that shouldnt be there.

           

          Also remember (BEFORE MANUFACTURING!) to do DRC and assert # of

          airwires=0 after ratsnest.

           

          1 of 1 people found this helpful
            • Re: mystery air wire in my project
              wilykat

              CadSoft Guest wrote:

               

              The VIA there is logically connected to that blue net, and I think it is

              not connected to the overlapping. Yellow cross means there is an

              vertical airwire between layers.

               

              Use show on the nets or vias and you will see the whole net highlighted,

              and maybe find connections that shouldnt be there.

               

               

              Using show, I noticed that the 2 vias for the power connector were both connected to VCC rail when one should be GND, that explains the air wire. Now to fix the yellow X's and check for sneaky air wires

            • Re: mystery air wire in my project
              CadSoft Guest

              On 05/09/17 10:16, Eric Chapin wrote:

              Can anyone explain the air wire between GND and VCC near the bottom?  Picture: https://imgur.com/on0AMd8 the pink arrow.  There's also a few yellow X's where the trace connects with decoupling capacitor pins, like Eagle doesn't know those traces are connected with capacitor's leg.

               

               

              As Morten said, that via is associated with the upper trace net, not the

              one it's placed over. If you move the via you should see that the

              airwire follows it, whereas if you move the lower diagonal trace (and

              the unconnected end of the horizontal bit it doesn't connect to) the

              airwire will stay still.

               

              1 of 1 people found this helpful
                • Re: mystery air wire in my project
                  wilykat

                  Yes I got it thank you.  I did manage to find one more sneaky airwire by typing in command "display none unrouted" which hid everything but unrouted.  All other unrouted are tiny and within the hole for component leg so it'd be connected when it's soldered in place.

                   

                  Checked top layer only for crossed lines, then checked bottom layer for crossed lines.   And finally ran error to find any more issue. Nearly all reported clearance issue with trace at vias and pads but those should be OK since they are supposed to be connected.  I didn't find any trace touching pad or vias where they aren't supposed to be.