How do I add links to the PCB layout?

Sorry I can’t upload the PCB file as I am still new?
I have a PCB that when I add a filled zone and connect it to the earths it has two zones that are not connected.
I can add a VIA to each zone with the intention of adding wire to connect them on the board.
I can route a track on the upper layer (the filled zone is on the lower layer) between the two vias.
I am sure there is a better way to do this, for a start if I look at the 3d of the board it just shows two holes and no link. How do I add wire links to the PCB page?

1 Like

Try now. and 20 more…


Hello, Bob, and welcome to the Forum.

Spend a little time reading a few topics, click some “Like” buttons, and the software will automagically increase your privileges. Or rattle the cage where they keep @hermit and the other moderators, and one of them may short-cut the software. Especially if you send them a serving of their favorite malt beverage. :beer:

I will confess that I don’t really understand your question. I am guessing that the answer is something like, "Be sure the tracks and vias you add are associated with the exact same net as the fill zones you are connecting. Then, hit the “B” key. (Keyboard shortcut for “Refill all zones”.) "

Side comment: According to tradition, convention, and standard practice the Gerber files are the ultimate authority for fabricating circuit boards. Open a Gerber viewer and see if what is shown, or not shown, on each layer matches your expectations. Don’t rely on anything else (3-D models in particular) for any Design Reviews, QC Audits, etc.

(OK, there are documented cases of certain Gerber viewers misbehaving, so perhaps you should check your files in TWO different Gerber viewers before you cry “Wolf!”. I don’t recall any instances where KiCAD’s own Gerber viewer, or the “Gerbv” viewer from the GEDA project, were proven to misbehave.)


1 Like

Thank you dale.
When a board is made and populated it often has bits of wire linking spots that the tracks couldn’t connect.
I have connected all the components in the pcbnew apart from the earths.
I have added a zone connecting all the earths.
There are two zones each connected to some earth points but not to one another.
I can add two VIA’s, one to each zone with the intention of adding a wire to the board to connect them. Can I add this to the schematic, so that it shows on the schematic or just to the Pcbnew? Is it possible to add it so it knows it is a wire link? (shows up on the 3d model).comparator3.kicad_pcb (58.3 KB)
It allowed me to upload the Pcbnew? can you see that?

Yes, we can see.

You have only the bottom (back) side filled with copper and no copper at all in the front side. No wonder there’s one unconnected area.

How is your board made? Will it be one sided? If yes, I can understand better your intention. If not, but it’s manufactured in a modern factory, make it two sided and just add another earth zone to the front side.

In a one sided board there are several possibilities. You can for example divide the earth net into two and add a 0ohm resistor symbol between them and attach a modified through hole footprint into it.

Can you tell more about your needs and restrictions?

BTW, the board lacks edge.cuts outlines. You have drawn only the zone polygon on the copper, but it’s not the same things as the board outline.


Thank you for the reply.
I intend printing out the board and etching it on to copper here, in fact I have already done so single sided and added a link between the two ground zones but I just wondered if it is possible to design a board with wire links added to the layout so it makes it clearer as a project?

When designing SS boards, I usually place tracks on top layer which represents wire links and keep DRC happy :slight_smile:

1 Like

Just like ZASto, I would use the top layer of the pcb to simulate the “wire bridges”.
While laying a track you can press the [V] shortcut to jump to the other side of the board and a Via is automatically added.
Also change your via size in:
Pcbnew / File / Board Setup / Design Rules / Net Classes
I see you already changed the track width for the default net class. Now enter something like 1.5mm for via’s with a 0.8mm drill size.

Laying out a board effectively also requires some “weird thinking” which you get by practicing.
For example, just by moving the track with the net “Net-(D1-Pad2)” to below C1, the connection is already made:

Also, by routing "Net-(D1-Pad2) around the connector pin 4 of the 5 Earth connections are no very close together on the same piece of the GND plane. Ideally you also want Pin 1 of the LM311 with a short connection to that same section of GND plane, without routing it all around the resistors.

For “good” PCB design a lot of other improvements can be made. I would at least add (room for) a decoupling capacitor between “Earth” and “+24V”,(100nF is usaly enough) and put that capacitor in between the connector and the LM311 and close to the IC.

Also: if you want a GND plane on a circuit, always try to make it in a single slab of copper. If you need to use wire bridges, then use the wire bridges for signal wires, and not to connect different parts of GND planes together.

I tinkered a bit with the layout.
Now I have a much smaller GND plane, but all the GND connections are connected solidly together.

I also made some other small changes.
First I made the outline of the zone look weird & crooked. The goal is that the outline of the board clips the edges of the GND plane, and if your generated gerbers look crooked you instantly know something has gone wrong.

Second: I drew a board outline on the “Edge.Cuts” layer: image This is the yellow line on the screenshot and it is what KiCad thinks is the

Some other notes:
Add some mounting holes to the PCB.
Check your resistor footprint size, they seem too big for “regular” resistors. Put one of your resistors on vero board or a breadboard, and then count the holes.

I also had a bit of troubles with the grid. The grid size is not stored in the .kicad_pcb file, and therefore my tinkering is a bit off from what you would expect.
This is what I came up with: comparator3.kicad_pcb (51.7 KB)

Thank you so much for the replies and the help you are giving me.
I can’t continue as the program seems to have crashed? I opened a new thread see
My PCB layout editor refuses to load?.
If I manage to get my problem solved I will return to this thread.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.