I made a footprint for a 6 pins SMD led. This led has actually 3 led chip built in so all pins on one side are cathodes and all pins on the other side are anodes.
I design road signs enhanced with LEDs and such those leds are placed all around on a grid less pcb.
Since I always make these leds run in parrallel I made a footprint using the recommanded pattern of SMD pads with no number, (actually a space). Then I made a very long and narrow pad to connect 3 pads on each side with no number again. I then placed 2 standard trough hole pads and these are numbered 1 and 2.
The reason for those pads is that saves me quite some time when routing as I don’t have to start a track, then change side until the destination point where I have to change board side again to join the pin on the component.
This works just swell without problem so far.
BUT… ( there is always something!)
For a design I am working right now, the leds are to be mounted on the bottom layer and the rest of the components will be mounted on the top side. So I ‘flipped’ the leds and placed them where needed.
When I try to route them, the router acts as if I had a rule violation and will not let me place tracks from the bottom side!!??
I have to start on the top side, run a little, then change side, which will place a via automatically, and continue routing the net until I arrive at destination where I have again to change side and finish the track on the top side.
I think I understand what is going on somewhat… It must be creating a rule violation of some sort or it acts like if wanted to start a track outside a component.
I must also state that when I click to start routing a net, I can see the net label as usual.
I must also state that I did not try with other component footprints.
As you mentionned bobc, “obviously” !
But that is not the problem.
I think the problem stems from the fact that it seems the track placement function does not ‘see’ the net starting point. And it works if I start on the top side.
This is really strange… LED_PLCC6.kicad_mod (1.6 KB)
Here is the footprint I made.
I assume the two THT pads are intended to be used as a replacement for vias?
If so they must have the same pad number as the pad they are on top of. (All smd pads of the footprint have no pin number assigned -> this means kicad does not allow a connection to them at all.)
In your case give all right footprints the pad number 2 and all left footprints the number 1.