Hello everyone, I have designed some projects on Kicad, but I feel blocked lately.
I wanted to design a “composed” footprint because I am designing an matrix for a keyboard. My footprint is composed of my switch, a diode and a bunch of copper trace. The issue is when I try to put actual trace on the hole, it throw DRC error… Have you an idea why I can’t make it work ?
The issue is not present when I try to trace on Front copper while the footprint is using back copper and the opposite
i don’t think that making it as footprint could work.
You should try using hierarchical schematics (and replicate layout plugin)
Aw you’re so fast I haven’t even had time to embed a picture ! thanks
I am using a plugin for keyboard layout that needs actual composant…
When making antenna what make the whole thing work in order to be able to root to the pcb antenna ? I thought it would have been the same
i see, well you can try removing net-names (row…) and see if something changes.
By putting the same number on the pads that are to be connected, when you do the layout the editor will require you to provide the traces. So you don’t need to (and probably cannot) put traces in the footprint.
Just to try I have erase the number on the top pad in order to have a logic behind having the trace
I can root from the trace but not from any hole even if there are highlight (I have changed in the footprint editor the Net field in the bottom copper trace that’s why it is greyed out)
No. Don’t do that. Keep the pad numbers, and keep them the same.
KiCad has no provisions for drawing tracks inside a footprint. I am guessing you have used graphical lines to connect the pads, and these graphical lines interfere with the tracks when you want to draw actual tracks on the PCB. A simple workaround is to remove the graphical lines in the footprints, and then replace them with SMT pads. You can remove the solder mask layer (and other technical layers) from these tracks so they get covered by solder mask, don’t appear on the stencil etc.
The pads for your diode also look weird:
Is this for an SMT diode? or to keep options open for either SMT or THT diode?
Why not? The Replicate Layout plugin is definitely worth looking into. It is by far the most popular plugin for KiCad, and I’ve heard some rumors that it (or it’s functionality) may get integrated into KiCad itself in due time, but I do not see a reason why this would not work.
You probably will get an ERC error or warning that pad 3 is not in the schematic symbol. Adding this pad to the schematic symbol and setting it to “no connect” should fix that.
Yes it was graphical lines ! Okay I think I will do this because it just a pain to link everything by hand ! thanks for the tip I’ll update the post if it works as intended.
Yes it is for smd Diode (actually from the Kicad default library) but it is double sided solder mask because I want to keep THT SMD and reversible ^^ (ergo keyboard design)
I don’t use Replicate layout plugin, because the keyboard layout plugin takes in input a keyboard layout json file and it is really easy to get a good keyboard from it !
Thanks for your answer btw !
Awesome idea thanks ! worked like a charm (even if working with SMD pad is… original ahah)
No DRC violation anywhere ! just a Warning due to PadStack (my strange double sided SMD pad but I will cancel it by duping the pad on the other side)
Thanks everyone, I ll close the post during the week if nobody add nothing !
(Update, it worked for PadStack )
