How do I change path segment?


I still get confused. Sorry. :anguished:

I am getting closer to where I need to be but I have an issue with Electrical Types. For instance, I can’t figure out what Electrical Type a pin connecting to GND should be. I can’t see why it would be Power Output or Power Input, and bit Passive and Bidirectional give confusing results - sometimes they seem to work and sometimes not. Here, Bidirectional does not:

In fact, KiCad thinks it is a Power Input.

What Electrical Type should I be using?

Note: this is a complete new project to get away from all that _rescued_ stuff :smile: (9.5 KB)


On your components, the GND pin should be Power Input. (GND is 0v, so it is a power input just like your other voltages are.)


Ah! :relieved: Okay! :thinking: I was thinking that 0 V would be going nowhere (because it’s zero). :star_struck: I’ll give that a whirl and see if I get any GND net on my pcb.


The absolute number assigned to a power rail is irrelevant as far as the physics are concerned. All that matters is the potential between two rails. So, you could rename +5V to be GND, and rename GND to be -5V, and it would be weird, but completely correct.


I went through the symbols I have created and changed the Electrical Type for GND to Power Input. Now I do a Rules Check and get this

I just don’t get this.
(1) Pin 2 on RC1 is not driven but Pin 9 on IC1 is
(2) Pin1 on U3 is not driven but all the other GNDs are
(3) I can’t see why Pin2 of U2 is not driven.

If I wasn’t already crazy I’d be headed in that direction. :tired_face: I am starting to believe that KiCad has something against me and is dreaming up glitches at random.:dizzy_face: How can a trace work in one instance and not at another?


See your previous post in this thread. Can you see what is different? (See your third sentence). ERC will check that the state of each of the pins at each end of a net are consistent. Just check what types are at each end of your net and whether they will connect together. Working through this logically should show you where the problems lie.

Learning ECAD is hard. As well as the Kicad documentation and the ‘Getting to Blinky’ series, this website has several good tutorials to work through. This section is about hidden pins and power flags might be worth looking at for some guidance your current problem. How to use power flags is not immediately obvious but fairly logical when you think about it.

I absolutely admit that I am no expert (and EDA is not my day job) but personally, I think you might find it helpful to run through a several complete tutorials like this from beginning to end. You will pick up a lot of hints and tips on the way and understand why certain things are like they are. If you run through the whole series you will have a better understanding of the goals and requirements of each stage of the design process. Whilst trying to get your pet project up and running is a good learning exercise, I think you would make quicker progress if you worked your way steadily through a good guide, making notes as you go and refer back to them frequently. You have to have a certain eye for detail and consistency to ensure the electrons actually go the way you expect them to… Best of luck.


I’m surprised at how many times you ask this same question, and each time you are given or referred to the answer yet you still can’t work it out for yourself. I’m not trying to be insulting but this is in fact one of the simpler things you will encounter while creating a schematic and laying out a board.

When a net contains at least one “power input” pin it needs a corresponding “power output” pin to “drive” it. GND is one net that almost always has “power input” pins and therefore must have one, and only one, “power output” pin. So you need to ask yourself “Where is the “source” of the power for this net?”. In this case it is the barrel jack. Either it’s pins need to be of “power output” type or you need to attach a “power flag” to the net, usually at the source. However, you have wired the barrel jack incorrectly so you should start with fixing that.

Use the same approach with both the “3.3V” and “5V” nets. Their source are the voltage regulators and we already had this discussion regarding the pin type of the regulator output pin.


Yeah! :rofl: I find learning it made more difficult by some strange actions of the package (see next post).
I have worked through Getting Started in KiCad several time, and it does get you started, but as I am finding out it leaves a lot of things unsaid. I appreciate that it would be, to say the least, difficult to put it all in one book, but it does get you started.

I was disappointed with the Getting to Blinky series, finding it ill constructed - the tutor often gets lost and speeds around doing ill-explained repairs he should never be actually doing, interprets jargon using more jargon, and goes racing around with mouse clicks that are too fast to follow (and doesn’t explain what he is doing while he does it). It was a nice try. :confused:

There have been other webpages I have had suggested and I have worked through them all. You are right, you pick up bits and pieces here and there and eventually get to see the total picture( in a fog :thinking:).

I will spend some time with the links you have provided.



Sometimes I think I have understood the answer but I haven’t got it right so I come back to the question. It’s not that the answer was wrong, it’s just that I didn’t get it right. :dizzy_face: Take the Electrical Type for pins for GND. Someone told me to make the pins on my Symbols Power Input and I did that, but it trns out that some of them have to be Power Output. Consider the standard (from library conn) Barrel Jack, one of these image shown as

This gets to me with all pins Passive. I edit this so that 1 is Passive and the others Power Output when I save it I get
and I have not option but to click Yes (clicking No achieves nothing). Clicking Yes saves it in RESCUE

If I load it from that library (in place of the original) I seem to get somewhere. Given some furthjer jiggery-pokery with the two power supplies (also now inserted from RESCUE although that is not shown in the schematic I get

This feels great. The Rules Test has come up clean. I must be getting somewhere :grin:. Hold your breath :no_mouth:. Let’s try a Netlist:
That’s It! That’s all I get on my PCB.

Please excuse me if I am a little frustrated and confused. :upside_down_face:

Their is something strange going on. If I open emphasized text my symbols library in C:\Program Files\KiCad\share\kicad\Library it does not have (for example) AP1117-50 in it. I must have some pathing problem. I will investigate.

Where did my symbols go?

I suggest you read this FAQ post again very carefully: Electrical type of schematic symbol pins
Especially the section about power pins.

It might also be a good idea to read a book or two about the basic of electronics. At least the simple stuff like what is current, what do we mean with voltage, how is power transmitted. And yes all of this requires the understanding of some basic mathematical models.


That link is very useful. Thanks. BTW I did a couple of units involving electronics in Ad. Dip. Eng (Mech.). Sadly the theory was teflon coated - like the maths. I only ever learn these things by doing. Since then I have worked my way through Boxall’s Arduino Workshop - well most of it anyway. I still go back and refer to it.


You need to use each of these buttons in order.

  1. Annotate your components. (Button1) [Essential]
  2. Run your ERC (Button 2) [Optional, but helps you avoid letting the magic smoke escape.]
  3. Associate each of your symbols with the relevant footprint. CvPCB (Button 3). [Optional only if you are using a fully defined component]
  4. Import your netlist (Button 4).[Essential to get to pcbnew]

You seem to have missed out (3).

See this FAQ

You can only skip this step if your component already has a footprint linked to it. Your Arduino and U1 have had footprints associated with them but you haven’t associated any of the other components with a land pattern. How is pcbnew going to know that you want to use a tiny 0402 SMD capacitor or a monster through hole electrolytic and therefore what footprint to put on the board? This is one of the advantages of KiCad - you don’t have to decide what component to use until you get to design the board. In other ECAD systems - e.g.
Eagle, you have to define everything up front.
This is how your CvPCB table looks in the project you uploaded earlier - you must have done something subsequently to get you Arduino symbol in but you can see it is largely unpopulated so there is no surprise that there aren’t many components on your board!

On a separate point, the stock symbols and footprints are not supposed to be edited but if you do edit for your own purposes, they should be copied into your personal library in your user space where you have write access.

This is now getting a long way from the original post.

And, furthermore you will run into a problem with your DHT22 symbol where you have defined the GND pin as passive.


Well this conversation has been spread over so many topics on this forum that it’s hard to tell who told you what. But if you go back to my last post I tried to make it clear that, although most of your GND and power connections will be of power input type, there needs to be one, and only one, pin of power output type to drive them.

Another case where I don’t know why these pins would be passive but, as was explained to you already, you have two choices. Either modify the symbol so that the pins are power outputs or add a power flag to the nets near those pins.

This is another one of those poorly worded messages. You either do not have permission to write to files in that folder or the files are write protected. Either way when modifying a symbol, or footprint, from the KiCad libraries you should not be trying to save your changes back to the KiCad library. You should instead be saving these changed symbols and footprints to your own libraries in your own folders, and then add these libraries to your project. There is plenty of information on this forum on how to do that.

And as I said previously, your barrel jack is wired incorrectly. If you look at the photo you posted as well as the symbol, that big fat thing attached to pin 1 of the symbol is the center post shown in the photo. You not only want to connect to that pin but that is usually the positive pin, you need to check with the adapter you plan to use. Pins 2 and 3 form a switch. When the plug is inserted the outer sleeve of the plug makes contact with the pointy part on pin 2 and pushes it away from pin 3. So with the plug inserted you have power applied to pins 1 and 2, pin 3 is open in this case but can be used to switch to a battery for example when the plug is removed.

Where did my symbols go?

KiCad will only list one error of the same type per net, there is no need to flag potentially hundreds of power input pins with the same error message.


That explains the numbering of the pins. It is a different interpretation of the ‘drawing’ than mine which had the ‘big fat thing’ as the pin on the side of the actual device, the line on the left as the pin in the actual device (+ve) and the other thing as the contact on the outside of the jack (-ve).

I suspected that, but it’s nice to be sure.

Any, after more reading and a fresh start I a pleased to report that I seem to be getting the hang of this because I now have


I agree with John_Pateman that “This is now getting a long way from the original post.” I propose to leave this where it lies. My thanks to all who have spent so much of their time answering my seemingly endless questions (even if it sometimes appeared a thankless task). I have to wait another couple of days for some parts to arrive then I can breadboard this circuit and iron any kinks out of it. I’ll be back when I get to putting traces and the GND zone on the board.

Have a great weekend.


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