Errors because of footprints in PCB editor

Hello, in my design several SMA connector is applied. Which cause some errors in PCB editor:

Here I believe that four ‘‘2’’ pins are just there to fix the connector on the board, but if I left them unconnected, errors will be reported.
Besides, I have already set those Pins unconnected in the schematic editor:
2,Another error is also reported:

I think it’s because of the outline of the footprints:

So is there any methodes that I could correct these errors ? Or maybe I could just ignore them ?
Thank you :slightly_smiling_face:

The shield of a coaxial connector is a critical part of the RF circuit and must be connected. These connectors use 4 pins to give as low impedance as possible to a groundplane.

Yes. The footprint you’re using has an Edge.Cuts line in it. The intention is for you to connect that to your board’s outline. If you don’t need or want that cut then you either need to use a different footprint or remove it from the footprint you’re using.

1 Like

Not sure why we have edge cuts in Kicad footprints ???
if the user needs something, put it on some other mechanical layer to use as a guide.
PCB design is not plug and play.

LF666, there are a number of gross defficiencies in your schematic and PCB, I suggest you go to a forum where there are people that can help you- and discuss there- that forum will have plenty of users to help you with your design - both electrical and mechanical. This forum is for Kicad specific problems and your issues are general - they would apply to any tool that you might use- , and are not kicad specific.


They were added for devices that sit in a defined aperture in the board. Examples include mouse optics and RF power transistors.

ahhh. OK. maybe the presentation in the footprint editor needs some enhancement if lots of people are coming array with this one.
Have you got a name of one with edge cuts I can look at in the std kicad library ? thanks - g.

Check Connector_PCBEdge:BUS_PCIexpress_x1 for example. This includes a partial board outline for a PCIe card

Note that some other footprints have PCB edge reference markings that show where to place the footprint so it overhangs the edge by the correct amount. These markings are not in the edge cuts layer, but rather in a user drawings layer (even though they are the same color in my screenshot)

Hi Jon , thanks and agreed .

Yes, a User Drawings Layer for a ‘partial outline’ is where I would expect to find edge cut guides---- The user can then draw their edgecut to suit.
That is, I would not expect an explicit edge cut to be supplied in a footprint.

But, I bring up the PCI express, and there it is, an edgecut on the edge layer. OK.
My comment is that in my system it shows up as the same default color ( another shade of grey) as User.Drawings, User 1., User.5 etc

Perhaps edge cut default color could be something that stands out a bit more.
However, “not a big deal for the user to change”

I can see the usefulness in the edge cut in specific circumstances.

1 Like

They are supplied when the edgecut needs to be precisely drawn relative to the rest of the footprint, and just supplied as guidelines in other cases.

if they’re only guidelines, they should probably be on another layer.
anyway, purely subjective commentry on my part, horses for courses I guess.

they are on other layers when supplied only as guidelines

1 Like

very good. thanks Jon

Hey, thanks for the response, what I need to do is to connect every ‘‘2’’ pins to ground ?

Yes all to a ground plane. Also try not to run other unrelated tracks inside the pins 2 area or you will get crosstalk.

1 Like

Don’t know the reason in this case but I frequently define complete enclosures as a footprint. Not only the edge cut but also the mounting holes, terminal blocks and a transparent model of the enclosure. So I cannot accidently move some of them and the terminal numbers correspond to the numbering in the device book. Saves a lot of time when you use this particular enclosure again. :wink:


Yes, seeing the blue cross ‘Not Connected’ on the the outer of the coax symbols made me think what ? :scream: this must be a unique use case I have never seen or it’s simply wrong ! I should check your schematic very carefully.

1 Like


I was Director of Engineering for Oregon division of JAE so, I saw this Connector with Edge-Cuts in the Stock Lib. I added the additional Edge-Cuts to the PCB after placing the Footprint…

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