Pad too close to copper item error, even when components are far apart

Hey Everybody, hopping all doing well. I am having an issue with Kicad 5.1.10, that I cannot wrap my mind around. I used to have this issue with more complex designs which did not cause any issue after production. But, now i have this issue in a more simple design and I decided to share.

As you can see in the image below, the message is saying that the pad is too close to a copper item. And that coper item is a SMD jumper. But, they are far a part but still getting the error. When I remove the component entirely the issue goes away.

I really do not understand what could be causing it. I am not using any custom component here. All coming from kicad. In other designs I was using some custom components which led me to believe that could have been the issue. But, now, I think there is something else here.

Thanks for the help.

According to your error message:

image

JP1 has a “Graphic Polygon” on a copper layer and this is very suspicious.
J2 is at quite a distance from JP1, so load the footprint of JP1 in the footprint editor (Or move the copy on your PCB to some empty area) and then have a close look at that footprint in the area that J2 is now.

Thanks for the reply @paulvdh. Is this what you mean?

About your comment in JP1, this footprint is actually done using graphics to draw the shape. Look below:

PS:. I had to put 2 comments because I am not allowed to add 2 images in one. Sorry about that

Can you just attach the board file here?

Euhm, almost but not quite.

And that you made JP1 (Did you make it yourself?) is made out of custom shapes confirms that I MAY be right.

I suspect that there is some extra polygon on a copper layer in JP1, that overlaps with the other footprint (J2) if you put it on a PCB.

If you can’t figure this out further, then I agree with eelik. Upload the PCB here. (You can delete all the other stuff, it just distracts from this issue, but make sure the error is still there)

Here you go @eelik. I should have started with that right?

https://drive.google.com/file/d/1Knw03dB5xrJw65L5t-MA_yCmzPqW1c4u/view?usp=sharing

I didnt make JP1. It is from a library SolderJumper. But, I just noticed it might be a thirdparty. But, the same issue also happens when I use a PCB antenna. Which is also a thirdparty (Texas_SWRA117D_2.4GHz_Right.kicad_mod)

I believe that adding the J2 to the error is a bug in v5.1.

For some things KiCad uses hacky workarounds and a net tie is one of them. Open the footprint in the footprint editor, add words “net tie” in the beginning of the footprint keywords and the problem goes away.

2 Likes

You did it. Thanks @eelik. Is there any side effect to this action?

No there shouldn’t be, it’s the official way to handle a graphic shape touching pads inside a footprint when it’s intended. A footprint which shortcuts two nets is a net tie, it’s not a solder jumper (the former is closed by default but may be cut, the latter is open by default but may be closed).

3 Likes

What I didn’t read that I don’t know that = where that (and probably other) official ways of doing something are written?

Unfortunately there’s no collection for those things (unless in the handbook which nobody reads anyway :slight_smile: ). This one I have read in various discussions here and there, maybe told by a developer. It may have been @JeffYoung who has been involved.

Implementing support for net ties as “first class citizens” was planned for v6 but it was postponed to v7. The current keyword hack is temporary.

The habit actually started in the official libraries – even though at that point it didn’t affect how KiCad processed them.

Later when we started doing more checks inside KiCad and the standard library components started failing those checks, we added code to look at the keywords.

So there might be some doc somewhere in the library team’s web presence. (Or maybe one person contributed all the net ties and they just happened to do it that way.)

A week ago I was designing PCB with RFID antenna. I didn’t used the conception of footprint for that but I just had a short at schematic and three circles made by track at PCB. I noticed that it is easy to lost all that work by accidentally going too close to it with another track - interactive router finds ‘better’ way to do that antenna.
Because of that I thought of preparing such footprint ‘for future use’. If I didn’t noticed this discussion I would never had write ‘net tie’ in Keywords. I supposed (was really sure) that it is only used if someone searches library for something. All my footprints has ‘Kaywords’ just empty :frowning:
The ‘net tie’ is the only ‘magic words’ or there are others?

I don’t know Python but I had to modify a little bom_csv_grouped_by_value_with_fp (it was 4.0.7 times) because listed references were not sorted. I ended with script that calls the Sort function twice and I don’t know why only one of them works as expected (each call is done a little different way but according to my understanding should work the same way). During reading that code I found that there are procedures to delete from BOM symbols that have field ‘Installed’ with value ‘NU’. So I have added that field to some of my symbols.
I think it is also undocumented feature.

“net tie” is the only magic word that I’m aware of.

(We planned on fixing it in 6.0, but “first class net ties” is one of the features that ended up getting pushed out to 7.0…)