I attempted to design an edge connector using the part Samtec_MECF-40-0_-NP-L-DV_2x40_P1.27mm_Edge, but it didn’t turn out as expected. The edges of the PCB were not removed as required, resulting in the connector not fitting properly. How can I resolve this issue in KiCad?
1 Like
You haven’t edited the edge cuts outline to produce the connector finger. The 3D preview shows the minimum bounding rectangle. Somebody else will surely chime in about the minimum radius for the concave corners for feasible manufacturing.
You might also want to look into chamfering the connector finger. This is usually an extra service from the fab.
I drew the edge of the PCB using the edge layer, and it passed the DRC . The issue is that when I place the default edge connector footprint, running the DRC shows errors
It is the edge connector that comes by default in KiCad
Merely adding that footprint does not magically extend your board outline to include it.
Draw your board outline around the line on the Edge.Cuts layer on the footprint, then edit the footprint (Ctrl+E) and remove the lines on Edge.Cuts.
That is one way of doing it, but you (probably do not have to modify the footprint itself.
But you do have to combine the lines from the footprint with the lines in the PCB editor in such a way that they form a perfect circumference for your PCB.
Lines on Edge.Cuts are not only used for the PCB outline, but they can also be used for internal cutouts and routing in oval pads. If you make it difficult for KiCad, then it just gives up and asks you to fix it to remove ambiguities.
It looks like that footprint from samacsys also has a line on Edge.Cuts on the top side of the edge connector. If that is true, then you will have to remove that line in the footprint itself. Footprints from externals sources such as Samacsys, PCB Libraries, SnapEda and such often have issues that have to be fixed before the footprint can be used in KiCad.
Which is what I said.
No, that is not what you wrote. You wrote:
You do not have to remove all the Edge.Cut lines from the footprint. You can combine a partial outline from Edge.Cut lines in the footprint with more lines in your PCB project. Several edge connectors in KiCad’s default libraries have a partially defined outline on Edge.Cuts, and that is normally supported in KiCad. It’s a subtle but important difference.
I extended the border using the edge cut layer after measuring the footprint and placed the footprint of the edge connector on the extended border. I then removed all other layers except the pad from the footprint. Since I am new to PCB design and KiCad, is this the correct method for edge connectors, or is bevelling of the PCB board edge also required?
If it renders properly in the 3D viewer, then you have to be at least pretty close, but to be sure, run DRC and read it’s output.
1 Like
Beveling makes the connector easier to insert, and may make the mating socket last longer, but isn’t strictly necessary. If you are only getting a few boards made, just chamfer it with a file yourself.
1 Like
Beveling of card edge connectors is very common, but you do not have to do it on the PCB. As far as I know it’s just an extra check mark during the ordering Process. PCB manufacturers know what beveled edge are for, so it will be unlikely the’ll bevel the whole PCB 
1 Like
If you select “Gold Fingers” at JLCPCB, you automatically get the option for chamfering presented.
1 Like
Don’t forget about this. The cutting tool has a small radius so the fab can’t make inner right angles; the corner should be rounded, or a bogdone, er dogbone.
1 Like