Right now, I am working with a surface mount USB Micro-B connector. All that I have found have suggested footprints that overhang the edge of the board AND require a pair of notches in from the edge of the board. The notches need to be located pretty precisely relative to a pair of tabs on the board side of the connector. I can see several ways of dealing with this:
(a) wait until the very end to create the slots based on footprint dimensions.
(b) add some construction lines to the connector footprint to show the desired slot position.
(c) add some sort of edge detail to the footprint so that the slots are created when then footprint is created.
I would really like to find a way to do (c) because, then, the slots would move when the connector moves. But, I don’t see a way for the open slot ends to over-ride the existing board outline.
The question, then, is: how have others resolved this problem?
Many thanks
Jim Wagner
Oregon Research Electronics
Some connectors have lines directly on Edge.Cuts and you have to connect further lines to it to get a complete PCB outline. USB_C_Plug_JAE_DX07P024AJ1 is an example of that. It is an apparently standardized card-edge connector:
Another method is to simply use a graphics line to suggest where the PCB edge should be. This is a better option if it is only the distance from a straight PCB edge. It also leaves room to wiggle a bit , for example to compensate for the wall thickness of an enclosure.
Just as an FYI, here is the sort of manufacturer’s footprint drawing that I am trying to cope with. The ultimate question is how to get the notches drawn as part of the board outline, and draw them in the correct position since dimensioning from footprint drawing elements to board drawing elements can be “challenging”.
I had a bit time left over and I was curious whether I would encounter any problems while drawing this in the Footprint Editor, and I did not encounter any problems. I just started by setting the grid to 0.05mm and then drew a line on Edge.Cuts starting from (-10, 0).
The depth of the notches did not fit on the 0.05mm grid, so after drawing the line, I selected the horizontal line segment, and changed the Y coordinate from -1.9 to -1.88, and then snapped the endpoints of the vertical segments to the endpoints of the horizontal line segments.
The pads were a bit of a nuisance, because KiCad wants center locations of pads, but the drawings usually have the edges of the pads dimensioned. So I used both a calculator I had on my desk, and added some simple formula’s in the entry boxes. For example for the Y coordinate of pad 1:
I only did the line on Edge.Cuts and the pads. You have to dress it up with silkscreen and other stuff yourself, (and of course verify my measurements). Verification is probably easiest by first calculating some coordinate with your calculator, and just looking at the properties of a pad or line segment.
I used rounded pads with the (default?) 25% rounding because IPC recommends this for more consistent amount of solder paste and easier release (paste can not stick to corners).
I also recommend to put some small THT pads through the mechanical pads 6 through 10. This makes the mechanical connection to the PCB much stronger.
Edit:
There is a bit of a gotcha:
The cutout notches are only 0.85mm wide, which is quite narrow for routing, and the square inner corners can not be routed at all. You probably want to modify this somehow in your final design.
I would be inclined to draw this one on FreeCad etc, with the “board outline” on one of the spare layers and then position it over the edge cuts and then trace over the notches in edge cuts.
Remember that the notches will be rounded as edge cuts is routed
However you do it, you can’t escape the tedious fine tuning after moving the footprint. KiCad requires strict continuous outline, no overlapping lines etc., so it’s impossible to do this automatically. Either you put the lines to an extra layer in the footprint and modify the edge cuts layer on the board, or you put the lines to edge cuts in the footprint and modify the edge cuts on the board.
Therefore I would suggest (a) and (b) together unless you really need the actual outline before the location and the whole edge is finished and fixed. If, on the other hand, you need the real outline for example to test mechanical compatibility with MCAD chassis, I would recommend putting the real edge to the footprint, because it would probably be easier to edit the board edge when the complicated part of the edge moves with the footprint.
for some reason, I think we’re had this conversation in previous post(s) - I say that because I’m in Oregon, thus somewhat remember your name. But, perhaps because we’ve met (maybe you worked for me ?)…
Anyway, here’s a link to my Video on how to do Edge-Cards… It uses Kicad 5 but, Kicad 6 now enables drawing the Edge_Cuts in the Footprint Editor so, you can ignore the info re editing the file (time range ~5:xx to 6:00).
Thanks to both of you for the comments and insight. I think that I will just put guide lines in the footprint and expect to tweak the board edge. I do understand the size and corner limitations; dealt with that a couple of times, already, on other boards.
Just saw your post recently. I am in the process of selecting a Micro-B connector. I’m curious as to the function of the slots in the board. Would you mind posting the PN for your footprint?
All of the connectors seem to requires those notches in one form or another. They all seem to have a tab or protrusion on the underside of the board for which the notches provide clearance. Don’t know why.
micro USB connectors have spring loaded notches to keep the connector in the socket. These protrusions go through holes in the socket, and may extend a bit below the PCB surface.
