Pad too close to copper item



I updated Kicad to 5.1 (running on Windows, if that makes a difference) and now I have new DRC errors on my board that I’m pretty sure I didn’t have before. I’ve looked around and found only references to the source code for the specific error on the title of this post (pad too close to copper item). In my particular case, the footprint is an PCB antenna loop that is terminated with capacitors. I placed two pads on each of the track ends, and placed one of the capacitor caps on top of them. See the screencaps below:

Part footprint

The PCB has some keepouts to avoid copper pours

Capacitor placement

As an experiment, I tried to remove the top copper trace in the footprint that connects pads 3 and 4, and the error disappears. That puzzles me because then there should be a similar error on the bottom pads of the antenna, pads 1 and 2.

Can you help me to get rid of this DRC error?


Why do you put the capacitor on top of another pad? That is at least strange if not dangerous.

How are these tracs made? Are they drawings on copper within the footprint or are they proper traces?

  1. I put the capacitor on top of the pad because I defined a rectangular keep out area. The keep out area prevents joining the antenna and cap pads with a track. I tested placing the cap on top and got no unconnected errors (or any other DRC errors for that matter) from either v4 or v5.0. The gerbers are perfectly fine and the design works. Could have defined a polygonal keep out area that didn’t cover the antenna pad? Sure, but the first try was simpler, and it worked, so I went with it. It might be quite unorthodox and not be the answer that you were looking for, but that’s the reason why I did it :smiley: As I said, the gerbers are perfectly fine, so I don’t understand what you mean with “strange” or “dangerous”. The biggest risk I’m facing is that I get a DRC error, but Kicad 4 and 5.0 was smart enough to understand that two pads that overlap are electrically connected.

  2. It’s copper defined within the footprint. As far as I am aware, all the PCB antenna components I’ve stumbled upon are defined as copper features in a footprint.

Also, I don’t understand why are the top pads triggering the error and the bottom ones don’t.


Could you share the antenna footprint?
Are pads #1 of C29 and the other top cap connected to each other in the schematic?
Maybe the antenna diagonal track on top overlaps the center of the pad of C29 while it doesn’t cover the center of the other pad and the DRC sees this track as “some unknown copper” touching the pad.


I checked the part, and the top copper is defined with a single line, on the top copper layer, drawn with the “add graphic line” command, while the bottom one is drawn wit the “add graphic polygon”. I tried replacing the graphic line for a polygon on the top copper layer and that fixes the issue. Why would the graphic line trigger it in the first place? I think that pretty much solves the issue. Can somebody tell me if that is the expected behaviour? If it isn’t I can create a bug report.

@Rene, would you have any suggestions about how should I lay this part out?


Here’s a library with two parts, one that tiggers it and one that doesn’t. The one called xxx_line_element triggers the (2.3 KB)


I’m having this problem too. It first appeared in V5.1.0, and is still present in V5.1.2.

If a footprint contains lines on copper layers, DRC gives an error if these overlap a pad. Prior to V5.1.0, it didn’t.

For various purposes like antennae and footprints for silicone buttons with conductive ink on the underside, it’s necessary to create footprints whose pads connect to copper patterns drawn with lines. Unfortunately until this bug is fixed, I’m going to have to continue working in V5.0.2 because my projects contain many such footprints.


Check the net tie footprints that are in the lib. They work with DRC and need the same basic thing.


Thanks! I just had a look though, and they all use polygons rather than lines - which as jsantosrico noted still works fine with DRC. Lines do not.

I was slightly mistaken earlier - the problem is more specifically when a trace (drawn in Pcbnew) intersects a line on a copper layer - rather than when a pad intersects a copper line, though the two cases usually go hand in hand.


Is there a way to disable DRC errors for tracks/pads crossing graphics areas on Copper layer (lines, not polygons)?
I’m using this type of feature for carbon contact keypads, but my footprints use Copper lines instead of copper Polygons. Why Polygons are OK for the DRC and lines are not? Is it a bug or intended behaviour? I’m currently on 5.1.2 stable.


The question is not why does DRC take copper lines into account. The question is why does it ignore polygons. (This is a bug by the way. DRC should check all copper features and it will do that in future.)

So how to do it properly? Convert your shape into a custom pad as that is correctly handled by DRC. And if you need a net tie, then insert one explicitly.


Great hint, thank you. Works like charm now.


I’m not sure if I understand you well.
Do the net tie can be used as part of antenna footprint?

I suppose not. Then the whole antenna footprint becomes being one pad. So you should have a symbol of RFID antenna with one pin and connect to it with one driving node and next through net-tie. Such schematic will be unreadable. Antenna symbol should have two pins.
If it is true (how I imagine it) then the right way in my opinion is to not use net-tie but to use in antenna footprint the same technic as in net-tie.


You can integrate the net tie into the antenna footprint. I am just of the opinion that making it explisit is a good idea. I also do not really feel that this would make a schematic anywhere close to unreadable.


May be we imagine this schematic differently.
Here antenna is a wire at schematic (I didn’t found the way in Protel to have it as symbol just because the same problem we are discussing here):

At that schematic I easily see that current is going through antenna coil.
But if we had a symbol with one pin and one wire connected to it directly and second by net-tie I would (at least at first moment) read it as one wire drives electric (not magnetic) antenna and second may be is a feedback, or from unknown reason two separate path are needed to drive the antenna - may be some signals are mixed in antenna. It would be for me very difficult to find that it is magnetic antenna. Till I will not find it I meen I don’t anderstand schematic.


Ah great, I hadn’t discovered custom shaped pads yet. With a bit of hacking of the file format I’ve managed to convert my old line-based footprints to make use of this.