So, long story short, I copied Eagle's standard RCL library to prune it down to the SMD essentials and to verify the packages. I removed the old library entirely, so it's not even loaded anymore, and loaded mine and replaced all relevant components in my schematic with a new version from my library.

Now, when I updated the schematic and told it to do a library update, it updates my board. That's fine. However, when I run a ratsnest, it unties the ground pads from the ground plane. What used to be 3 "prongs" from the pad tied to ground from the ground plane is now a single "prong that isn't even fully attached. Also, the ground plane will no longer run between the pads like it would before on the top side... and it puts a hole in the ground plane on the other side of the board.

I'm completely baffled on what would cause this. It's happening consistently with the packages I've modified. The only things I've changed are: updated pad sizes, moved the outline of the actual part to the Dimension layer, and added a courtyard in both tKeepout and in tPlace. I tried removing the courtyard lines from tPlace/tKeepout to no avail.

Here's a picture of what Eagle is doing:

good vs bad ground plane connection

Please help. I'm so friggin' baffled. :(


1 Answer 1


So, this seems like a silly thing, but apparently if you have something in the Dimension layer (which is where I drew the actual component), Eagle thinks it needs to be routed around. The problem was solved by pushing everything into the tPlace layer. Not ideal since I don't want component dimensions mixed with my courtyards, but I can figure out a way around that, ideally.

  • 1
    \$\begingroup\$ Yes, dimension is basically where your board outline (including interior drill holes) should be... perhaps you could use the Measures or Reference layers? \$\endgroup\$
    – vicatcu
    Commented Jun 21, 2012 at 4:05
  • 1
    \$\begingroup\$ I'm using tDocu at the moment, but a lot of stuff seems to use that for things I want on the board like courtyards, etc... so now I just have to clone and audit other packages. But yes... after looking... it seems I have many options to choose from, Measure and Reference among them. :) \$\endgroup\$ Commented Jun 21, 2012 at 11:36
  • 1
    \$\begingroup\$ If you are drawing component outlines then the tPlace layer is probably the most sensible. \$\endgroup\$ Commented Jun 16, 2015 at 20:20
  • 1
    \$\begingroup\$ And I realize this is an old question, but readers may be interested in looking at how the CAM process will interpret Eagle's layers. Look for the CAM files used by board houses that accept Eagle pcb files directly, and also look at the CAM files provided with Eagle. I recently tabulated this for one particular board vendor: grahamwideman.wikispaces.com/Eagle+and+OSHPark+layer+use \$\endgroup\$
    – gwideman
    Commented Aug 8, 2015 at 6:25

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.