I have created and had manufactured a board using the schematic and pcb layouts shown below.
On testing the board I’ve found that the DCIN pin of the IC is not connected to the DC supply. On the schematic it shows that they should be connected and in Pcbnew the DRC runs fine without showing any errors or unconnected pins, but on the board they are unconnected.
In short the DC supply should go through a diode and then directly to pin 15 of the IC which is the IC’s DCIN pin.
Here is the schematic.
(taken out - only 1 image per post for a new user)
Here is the layout in Pcbnew.
(taken out - only 1 image per post for a new user)
And this is a zoomed in version of the relevant part of the layout.
I’ve tried exporting the netlist again and re-imported it into Pcbnew. I’ve tried viewing this in Default and OpenGL. I’ve tried turning off all layer renders except for the Ratsnest but still nothing is showing as an error or as an unconnected part of the board.
Unfortunately as a new user I am only able to include one image in a post so I have taken two images out and have just included the zoomed in part of the layout.
Darren, open your schematic in Eeschema and zoom in by a few hundred times on the connection I marked on the atch image. (Park the cursor over that short “wire”, then beat the “F1” key about 8 or 10 times should do it.)
Look carefully, and make sure the “wires”, as well as the “junction dot”, actually DO touch each other. You’ll probably find a tiny gap separating the wires and/or junction. (In fact, the junction dot looks suspiciously fuzzy in your screen capture.) Extend a line, or move the junction, or re-draft that section of the schematic as needed to correct the gap.
A gap between connections can often be traced to changing the “Grid size” part way through the drafting process, especially changing between metric and English units. (See Preferences > Schematic Editor Options > Display ) Don’t ask how I know where this kind of problem comes from.
And, in the meantime, you have a stack of boards that need to be manually re-worked with a “white-wire” jumper to be usable. Within the last week or so there was another Forum post on the same topic. I think the discussion had more information about how to avoid the problem in the first place, but I can’t put my finger on the thread for some reason. Your search may be more fruitful.
I’m glad we could identify the problem so easily, and point you toward its solution.
To find if a junction sticks or not or a pin is attached to a wire do this test: #Hold mouse cursor over junction or part, hit [G] and move it a bit… any wires that are attached will rubberband-follow your movements… any that are not connected will stay.
Abort by hitting [ESC].
Just a friendly heads up: in the schematic, I noticed that you have a single net with two different netnames / local labels (in the top- and bottom right, ICHG/EN and REF) I recall there being some issues with prioritization and/or checking for double net names. You might want to change that if you want to avoid any other undesired / unexpected behaviour. Check if everything is connected as intended if you leave it like this.
