Footprint Pin won't connect

Layout
1

Kicad ver 5.1.5-3.
Downloaded connector footprint from manufaturers site, link below… Ratsnest correctly indicates the destination for the pins. However I cannot connect to any of the pins when routing, either starting the trace at the pin or ending at the pin. I have looked at the footprint but cannot find any errors with it. Anyone have any ideas please.
I have made many footprints and also imported many in kicad but this stumps me.
https://www.cuidevices.com/product/resource/pcbfootprint/pd-40
Any help would be appreciated.
Thanks
Paul

2

The battery of my crystal ball died and it needs recharging.

Maybe we can try it the old fashoned way:
Can you make a simple KiCad project with for example a schematic with 2 components and a PCB with your troublesome component that won’t connect and post it here?

3

Thanks for the reply. Battery for your crystal ball uploaded. This is the cct with all the other components and routing removed, just leavingSCH.zip (192.8 KB) 2 components.
Thanks

4

Found it!
Opened the PWR-DIN-4 Footprint in the Footprint editor and show the pads in “outline mode” (on the left toolbar).

image
image912×473 83.3 KB

The rectangles in the pads are on the “edge cuts” layer.
This means that the center of the pads is outside of the PCB and therefore can not be reached for starting or ending tracks.

When I start a track from the soic, and then route it as far as it will go to the connector, there is sufficiently overlap for DRC to accept it.

image
image929×532 81.6 KB

1 Like
5

My guess is that these shapes on the edge cuts layer are there to make oval plated holes. In KiCad there is a much better way to do this. Remove the edge cuts outline and select an oval hole for the pads.

6

Thank you both for you quick response and help. Ive changed hole to oval and deleted the edgecuts rectangle. At the least this will remove any ambiguity of being plated or not.

Thanks again

7

Apparently not all PCB manufacturers support Oval holes, or routing before electroplating, or there is an extra fee for it.
You may want to check this while placing an order for your PCB’s.

8

Good point. If I remember JLCPCB are ok (fro the first 5) - they are cheaper for multilayer then PCBway. The rest are being made in the UK so will check. Thanks

P

9

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