It is not clear from your post if this is a PCB that was originally designed in EasyEDA and which you are updating or if it is a design that you have recreated from scratch in EasyEDA.

Since all footprints and schematic symbols are public in EasyEDA, please identify it clearly in the Library and post a screenshot that includes the whole Library window.

Please do the same for the schematic symbol associated with it in the schematic.

The quickest way to solve this is to see your project.

If you can, please make the project public and post the url to it back here.

If not you could add me (andyfierman@easyeda.com) as an observer to your project.

@andyfierman Thank you for your reply!

The PCB was originally designed in EasyEDA.

Footprint:

Symbol in schematic:

Unfortunatley, I am unable to share anything beyond these screenshots. Thank you so much for the consideration.

Can you identify the switch symbol in the library?

Another thought.

Can you make a dummy project that just includes tge switch and the nets around it and a PCB made from it that demonstrates the issue?

Then share that?

@andyfierman Great idea. I have shared that with you. Thanks a ton.

@melbourneandrew,

Can you post the url to it?

@andyfierman https://easyeda.com/editor#id=574ae54f16654611acf126822a3d8036

Ah!

Got it: you added me to the project.

I can see that now.

:)

Based on your example, the short answer is that the footprint has been created to be placed ion the top layer but has pads only on the bottom layer so your top layer surface mounted components cannot connect to them without adding vias to swap layers.

However, I don't understand how in your original design the pads appear to be on the top layer along with D3, D6, R4 and R57.

The longer answer is that the footprint is not well constructed. It does not conform to the requirements in this How To:

https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6



The quickest way to fix this, is to edit the footprint to add a second small, single layer pad to each of the 6 pads. They can be round or rectangular but small enough to place at the outer end of each of but inside the boundary of the exisiting recyangular pads. The new pad must have the same number as the pad it is surrounded by.

To avoid it snapping straight ot the original pad centre place the new pad outside in the Footprint Editor canvas then reselect it and drag it where you want.

Then when you do right-click Update on the footprint in the PCB it should pull in the edited version and the tracks should be able to route to the new secondary pads.

Another, tidier but more complex solution is to rebuild the existing pads as polygons but manipulate the points so that the effective pad centre is offset to one end to move the snap point out of the Solid Region set to Cutout.

If you can accept having pads on both sides of the board with plated through holes (which is actually the correct way to make footprints for through-board pins), then rebuild the pads as slotted rectangular or oval multilayer pads and delete the Solid Regions used to form the slots in the pads (keep the one for the centre line slot).

Try to get the datasheet for the switch so that you can check the footprint dimensions anyway.

Then for your own sanity, do the essential checks in (4) and (6) in (2) in:

https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a

Ideally read all of it and the linked documents but you may not have time to get through all of it.

:)

Questions? Just ask.