How do I change path segment?

Rick, using only a text editor it is plain to see that there was indeed a pad named “GND1”.

(pad RST thru_hole circle (at 7.62 -10.16) (size 1.524 1.524) (drill 0.762) (layers *.Cu *.Mask))
(pad GND thru_hole circle (at 5.08 -10.16) (size 1.524 1.524) (drill 0.762) (layers *.Cu *.Mask))
(pad GND1 thru_hole circle (at 2.54 -10.16) (size 1.524 1.524) (drill 0.762) (layers *.Cu *.Mask))

I am sorry, gents. I don’t have that version any more.
I guess it just goes to confirm my wife’s suspicion that I am not perfect.
Mea Culpa!

Symbols are not supposed to look like the pin/pad layout of Footprints.

Symbols should have inputs on the left, and outputs on the right. It makes reading the schematic so much easier later on (when you learn how to read a schematic).

In the example I uploaded, because I’m managing my time in this thread, I did not move the ADC pins to the left side of the symbol. However, it is my opinion that the ADC pins (in general) are more valuable as inputs, and I would swap them over the left side of the Symbol as meant for a “generic” library Symbol.

1 Like

Yeah, mine keeps a list of “Things My NEXT Husband Won’t Do”. Of course, I have one for my next wife, also. Coming up on 44 years, and I think we’re both working in Volume 3 or Volume 4 of those lists.


Most microcontroller (uC) pins have several possible functions. You would not believe the INCREDIBLE number of ways a particular uC might get used in various projects! Consequently, I think I have created a custom symbol every time I have used a uC in a project, with the pins grouped and named according to how they are used in that particular project.


1 Like

And, that was the point. I currently value ADC ins over digital outs for what I’m currently working with. At the moment, it would save me design time to start out with them on the left.

Of course, that might change by Tuesday.

For me it also helps in understanding schematics to make custom symbols.
Vcc connection on the top.
GND connections on the bottom.
Signal flow from left to right.

This just looks weird:

1). Edit the values of your CP1_small to the values of the capacitors.
2). VDDA is probably some power connector, where is it?

I tend to make a nice section where all functionality of the power supply is grouped together in a logical way.
Input connector, buffer & decoupling caps, voltage regulators, PWR_FLAG labels.

But it takes effort and time to make those things a habit, and you have to start somewhere.

1 Like

Adding my 3 cents. I use one symbol for microcontrollers like that. Than I connect all its pins (except unmovable VCC,. GND, crystal, ISP/PDI) to one bus and name each net in the bus with function in current project. At the last stage of PCB design I change many pin function many times (to allow all my connections be on top with bottom be uninterrupted GND). That needs only to move net names betwean symbol pins and not changing the symbol itself.


It’s fair to say that I am having difficulty working out how to show power supply to a circuit. If this is not right, what is?

You need some physical part to get power into your pcb. Most likely this will be via a two terminal connector. If this is the place simply add a conn_01x02 symbol and connect it to the connector footprint of your choice.

1 Like

To further expand on Rene’s advice, put the power flag for the VDDA and GND nets connected closely to the connector symbol that you plan on using. This adds documentation to your schematic that the connector is the source of VDDA and GND. (KiCad really doesn’t care, but careful placement of elements like this in your schematic will provide self documentation. Much like properly chosen variable names when programming.)


As this project develops I have found the Barrel Jack I need and included it instead of a generic power source. This created an error rather than a mere warning! :confounded: (17.4 KB)

I have put Power Flags next to the connector symbols I use.
Mysteriously, Pin 2 on J1 (the Barrel Jack) is not connected to Pin 1 on anything. This is wierd! :thinking:

If the pin of the connector is already a power output you do not need another power output on the same net. The power flag is simply a one pin component with its pin type set to power output.

The power flag has a single pin with pin number 1.

[quote=“Rene_Poschl, post:33, topic:10711”]
If the pin of the connector is already a power output you do not need another power output on the same net.[/quote]
Okay. Because I defined Pin 2 of the Barrel Jack as power output I don’t have to do it again. I had defined Pin 1 of the Barrel Jack as Passive so putting a power flag on it didn’t help much. I removed both flags.

Of course! :blush:

The design evolves

and gets a clean bill of health but the Netlist does not include the Pro Mini or the sensor or the radio breakout

as shows in the PCB

The PCB puzzled me with the Spider Web Traces but the right things are connected to the right things - except for GND which is not connected anywhere. What classification should ground pins have? I have been making them Passive. (20.1 KB)

Sometimes I am so dumb I could kick myself! :weary: Perhaps I should have figured out all by myself that if certain footprints were missing then the best way to deal with the problem would be to attach them. :thinking: In this case I had to draw one of them. :sweat_smile: Anyway, that penny dropped. Sorry to have even mentioned the problem. :neutral_face:

There is more poking around to do. I don’t know why, but you are still missing your GND net. Even if you have a fill (which I doubt) and you have the fill not showing, you should still see the name of the net on all the ground pins. They all look conspicuously empty to me.

I don’t know if it is the source of this, but you have a major problem with your schematic symbol for the nRF24L01+ module. You have multiple pin number 1 and 4s. Reading the pin numbers in what looks like it makes sense, you have numbers 1, 2, 3, 4, 4, 6, 7, 1. The second “4” (SCK) should probably be a “5” and the second “1” (IRQ) should probably be an “8” and have a no connect symbol. But I don’t have the datasheet for that module on hand so you should double check that.

That’s because the GND symbols that appear in his schematic are not the GND symbol from the KiCad power library. They are the symbol GND-RESCUE-RemoteWeatherStation from the library RemoteWeatherStation-rescue.lib. In that symbol, he has marked the pin as passive. Therefore, he has a symbol which looks exactly like GND, but does not create a global net.

Thanks. I don’t know how I missed that.

I don’t know why this rescue.lib got created but I suspect it has something to do with being unable to write to the power library. I think KiCad creates the rescue.lib to hold edited version of the footprint. Going to the power library in Windows Explorer and giving myself read/write permission seems to work once but it then reverts to Read Only.

Not really. You can read about rescued symbols here. (And it’s not a footprint.)

Let me start by suggesting that you shouldn’t be modifying the power library. Use the power symbols as they are, and don’t change them.