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 donât 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)
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.
Thatâs some pretty tight spacing with those traces. Couldnât you flip part of the RX1 and TX1 trace to the top layer (then drop them back down once youâre out of the connector footprint?
Is it possible to âbump outâ 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 knowsâŚ)
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 âSCL1â and âSERVO_OEâ tracks go ânorthâ 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 OPâs 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 âBeginnerâs Guide to PCB Designâ - so to speak - that you would recommend? Thereâs 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. Iâm 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: https://www.pdfdrive.com/search?q=pcb+design
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 âGettiing started with KiCadâ guide a lot. (Included with KiCad itself) But itâs 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, itâs 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 youâd care to read. Iâm 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 - youâve shared an enormous amount of knowledge, such that Iâm going to print out the whole thread and keep it for reference.
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 donât have any other way to add plating (I donât 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 âAdvanced beginnerâ . 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
Youâre at a university, and youâre there to learn I presume?
But itâs 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 viaâs, 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. Iâve build complete PCBâs 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.
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.
