Indicate that pins in header will be connected externally

I am working on a PCB that will be connected to a Raspberry Pi compatible pin header, in particular a NVIDIA Jetson Nano. This pin header has a total of 8 different ground connectors. On the actual Jetson Nano PCB, these connections are all linked together, so I do not have to connect them in my PCB.

However, I cannot figure out how to indicate to Pcbnew this is the case. The end result is that I get a message indicating that the ground pins are not actually connected. Is there a way to indicate to Pcbnew that I don’t need to connect these pins with a trace on my PCB?


Minor Edit: After reading some comments, I realize that I was not too clear on some details about the question. I am aware that GND pins should always all have connections (see my reply in the thread as to why I am leaving some GND pins unconnected in this case). This is mean to be a more general question about telling KiCAD that specific pins that are connected in the schematics do not have to be linked in the PCB design)

Ground connections are important.
All your signals depend on it, and it also is the return path for the power.

There are multiple GND pins on the connector for good reasons.

Connect all GND pins on both side of the connector to GND, just as with IC’s that have multiple GND pins.


If you are trying to design a commercial product, looping ground return through headers is a good way of failing EMC tests for CE marking, for reasons @paulvdh gave.

A point about your screenshot, I try to centre tracks like between pins 8 and 10 to maximise clearance. It reduces production shorts.

1 Like

That’s some pretty tight spacing with those traces. Couldn’t you flip part of the RX1 and TX1 trace to the top layer (then drop them back down once you’re out of the connector footprint?

Is it possible to ‘bump out’ part of that pour to make room for a trace big enough to ensure electrical continuity between the ground pins?

Looks like perfectly normal PCB with pretty coarse design rules to me.
Just the easy one track between two 2.54mm headers (Although it could be a 1mm header. Who knows…)

But there are very likely much more pressing issues.
Just the question for wanting to not connect GND pins on the PCB makes it instantly clear that OP is a beginner with PCB design, and thats all right. Everybody has started at some time in their career.

A more important issue is that the “SCL1” and “SERVO_OE” tracks go “north” and by doing so cut right through the GND plane, while that other (red) plane seems continuous.

The screenshot is much too small to draw any conclusions, but if I try none the less and extrapolate from OP’s firs question, then I guess that the GND plane is cut to bits and pieces all over the PCB.

Paul, I too am a beginner, and your comment immediately struck a chord. Is there a “Beginner’s Guide to PCB Design” - so to speak - that you would recommend? There’s plenty of stuff online, of course, but the challenge is finding a trustworthy source of knowledge.

I can not recommend a book. It was over 30 years ago that I would have wanted such a book. I’m also not a professional PCB designer, just a hobbyist with a passion for Open Source software. I scrambled the info I know together from bits and pieces over those years.

I had a quick peek at:
A bunch of books relate to learning a program. (KiCad, eagle, orcad, pcad and man more) Those kind of books is not my thing. I did like the “Gettiing started with KiCad” guide a lot. (Included with KiCad itself) But it’s a short manual you can read in 2 yours and it gives you the basics of how KiCad works, and I prefer to fill in the rest of the details by just experimenting, which works quite well in KiCad and many other GUI programs. Unfortunately that guide is seriously out of date.
For learing to design a PCB you need another sort of book however.

Reading more about EMC (Electro Magnetic Compatibility) is a must, it’s the basis of what to do and what not to do.

Then there are books about specialized subjects.
From high speed digital design to High power electronics such as motor controllers.

It must be overwhelming to live in this modern world. When I wanted to learn something about electronics, you had to go to a physical store and buy a book or to a library, and make do with the few books they had available. The Internet did not exist back then. Even EMC in general was not a very widely known issue. That got really started when the EU decided to make EMC testing mandatory. Lots of books about EMC began to sprint up then.

That search on pdfdrive gives more related books then you’d care to read. I’m old fashioned and treat such sites as a library. Download a bunch, spend 15 minutes on a book to find a related an interesting topic, and if it does not work out, try the next book. If you find a book that has value to you, then spend more time on it.

Maybe you find this old thread useful: Seek review my first design I did a review of a quite simple beginners PCB. Maybe I exaggerated on some points, as I probably paid too much attention to details for such a simple low-speed PCB that is extremely unlikely to get even in the neighborhood of an EMC test. But it has some good tips about improving PCB design.

Thanks for such a detailed reply, Paul - it is much appreciated!

Also, the link to the old thread is extremely useful - you’ve shared an enormous amount of knowledge, such that I’m going to print out the whole thread and keep it for reference.

Thanks again! :slight_smile:

Rather than books I recommend manufacturers application notes
These two are good:


I agree. I am in the process of doing that and forgot to adjust that one before the screenshot. Frankly I do it for the aesthetics as much as for practical reasons.

Normally I would. the issue here is that this is a one off board for a university robotics project, and due to time and financial constraints we are using the PCB mill that the university already owns (since we can make PCBs for free with it with a 1-2 day turnaround and one of the project members is also one of the mill operators).
However, the university mill will not add copper inside the drills it makes (or do solder masking for that matter) and we don’t have any other way to add plating (I don’t know all the details, but I was told it was too expensive for the university by a couple of professors) so every via has to have a through hole lead soldered in it, and adding solder underneath a 2x20 pin header for stuff on the top layer is not fun. All of the other headers on the board do have traces on the top and bottom to simplify things.

Its a 2x20 2.54mm header. Standard Raspberry Pi Pinout.

I have done a few designs before, always for one-off school projects or hobby stuff (so CE/FCC cert is not a huge deal for me) so I like to say “Advanced beginner” . Normally I do connect all GND pins, but for the reasons I explained above, (and as at the request of the project member handling soldering), I have been trying to reduce PCB traces on the top half. I have been using a trace/pour on the top half, but with the knowledge that not all on that side might be connected.

The question was not really meant to focus on the fact that I used the GND net. I simply picked that as an example since that was for this specific case. My apologies for causing confusion. I have updated the question to clarify this.

Commenting on the original question, KiCad has no direct way of bridging a net off board. This is more often a problem with wire jumpers and parts with internally linked pins like TACT switches.
One way to cheat is to add extra copper layers with these virtual tracks (only!) and remove them again before generating Gerber plots

Darn. Oh well. Thanks anyways.

The temporary extra layers trick does work and allows you to run DRC before deleting them

You’re at a university, and you’re there to learn I presume?

But it’s more of a personality thing.
Some people do the least they think they can get away with, while others always do the best they can.

If you have to work within the constraints of milled PCB without plated via’s, then the trick davidrsb mentioned is a good one.
Just add an extra layer pair (copper layers always come in pairs in KiCad) and dedicate them to drawing wire-bridges only. And then of course also use it as a guide while actually building the PCB, so you do not forget wire bridges.

For wire bridges I prefer to use lacquered wire, and preferably use it with two soldering irons. One soldering iron is set to 450c to burn of the lacquer and tin the ends. The other is set at a lower temperature and used for the actual soldering. I’ve build complete PCB’s this way on perfboard and it is a lot quicker compared to stripping plastic coated wires. I use 0.2mm for low current signal wires, and 0.5mm for PWR & GND.

When I said darn. I meant that darn there is not a built in way to simplify for kicad. The trick does indeed work fine.

Hey Marsfan,

It is always a good practice to connect your ground pins even when the NVIDIA Jetson Nano has all the connections linked together. This will help you in case the connectivity of any of the pins is lost. And if you do not wish to connect them at any cost, you can simply remove the connections from the schematic itself and you will be good to go.

Paralled GND connections reduces the inductance and therefore the noise generated by signals between the boards.

I’ll add a few comments, mostly echo-ing what is above, but with the obvious question answered.

  1. You indicate that a pin has no connection by placing a no connect flag. Its a flag/symbol like any other.
  2. That said, i agree that multiple ground connections are desirable for two reasons: 1) proximity, shortest return path and 2) redundancy
  3. In some designs you may wish to keep grounds independent -such as I do for all low level analog vs digital grounds

So now you know how to be cheap and dirty, and why you ought not.

I also advocate at least two vias for any layer jump. 3 is better.

… and generally the largest trace, biggest reveal, and most continuous ground plane possible.


For No 3, you can give the pin on the daughter card a new name like GNDA.

… of course. In fact all ground nets ought to have clear designations, assigned before the PCB layout is conceived.