[KiCAD 6.0] When execute the command of "Update PCB from schematic...", warnings and errors, which are "No net found" & "pad *** not found", occur

When execute the command of “Update PCB from schematic…”, warnings and errors, which are “No net found” & “pad *** not found”, occur. The details are as following:

Warning: No net found for symbol DL1 pin 1.
Warning: No net found for symbol DL1 pin 2.
Error: DL1 pad C not found in LED_SMD:LED_0603_1608Metric.
Error: DL1 pad A not found in LED_SMD:LED_0603_1608Metric.

We are quite sure that DL1 is connected to R1 and GND.

We’ve created a simple demo project for this issue, but it cannot be uploaded since I am a new user.

SimpleDemoForPCBUpdateErrors.zip (8.9 KB)

Just read a few more postings or FAQs and you will be able to upload files.

I think that your pins need to have numbers assigned and not letters? It sounds helpful to have pads C and A for a diode, but I think you probably need to have pads 1 and 2. Other forum contributors: Am I correct?

Yes, this often a problem with symbols and footprints from non-KiCad libraries.

BTW @BobZ there are two Reply buttons. The one below the post replies to that post, while the one at the bottom replies to the thread. Not that it matters to me if you reply to me rather than the OP, since I don’t have notifications enabled.

Alpha-numeric pin designations would be a good “nice-to-have”.

Yes I am aware of that but I may sometimes hit the wrong one. This last post was intended to reply to you.

Years ago, business cards used to have phone and FAX numbers. If you were to bet against me when I am attempting to call the person, you could have made money by betting on me unintentionally dialing the FAX number and being greeted by the usual FAX answer tones.

@retiredfeline trying to figure out what is your avatar. I think it includes a cat but cannot figure out the rest of it…

Fixed. Try now. :wink: .

Wire between R1 & DL1 has two different widths???


I was not so aware of this capability but I can do the same thing. I guess it does not affect connectivity, and it is reasonable that it might have happened as a result of poking around to figure out what the software is doing.

It was just an observation. Maybe the thick wire is hiding something underneath?

OK as an experiment, I took a dummy project and added resistor R2. I used the symbol editor within the schematic editor to change the resistor pad NUMBERS to A and B. I get an error because my footprint has pads 1 and 2; not A and B. I feel 90% confident that this is the issue which @huskier has encountered. Please ignore the other warnings in my screen shot; this car of mine is not planned to hit the road anyway…

image

BTW I note that the original schematic image has a ground symbol rotated 90 degrees. Along with my comrades we used to complain about my manager at the time doing that. If this were a movie, we would all be pressed against the wall by the force of gravity and would be unable to get off the wall. :slight_smile:

Sent you the explanation by PM.

IIRC this already exists, I seem to remember that BGA pads are labelled according to a grid. As long they match up with the pin “numbers”, they will work. The problem is with some symbol and footprint suppliers that think labelling the pin Vin, Vout, GND, etc is helpful, but then the package is say TO-223 and the pads are labelled 1, 2, 3 so it’s no good.

Yes right. I think my earlier post is mistaken. Basically the pad numbers on the symbol need to agree with those on the footprint. I am unsure what other restrictions there are. But if I were just now setting up my KiCad libraries, I might assign pad numbers of K and A to my diode footprints and diode symbols. However after using the footprints in other designs already, I do not want to change my standard library now. Changing these would introduce errors in my pre-existing designs if I ever updated them to the changed libraries.

Yes, that is the problem. We’ve solved it. Thank you. @BobZ @retiredfeline @hermit