5
\$\begingroup\$

So, I'm trying to make a circular pad for a project:

enter image description here

To try to make my life easier when changing inner and outer diameters I created a package which consists of 2 pads: one horizontal, which connects one "fin" to the next one, and a vertical one, which is the fin itself.

The "origin" distance is the radius of the pad.

enter image description here

My problem is, I don't want the "unrouted" yellow connection between the pads since they're already touching, and the Package editor doesnt have the route command.

Is there a way that does not involve using the "wire" command and trying to guess the pad center? (I'm not sure if even this would work).

enter image description here

p.s.: I know if I just ignore the request to route it, I'll probably be fine. But I'd like to know if there's a proper way of doing it.

\$\endgroup\$
  • \$\begingroup\$ For something like that, I'd consider writing a program to output the desired geometry as an eagle file or inclusion thereto. \$\endgroup\$ – Chris Stratton Aug 14 '16 at 22:34
  • \$\begingroup\$ @ChrisStratton -- I understand this is somewhat of a brute force path. I have to learn writing scripts for eagle eventually. If you have any particular learning resources (URLs, etc) to recommend I'll take a look into it. \$\endgroup\$ – Wesley Lee Aug 14 '16 at 22:40
  • \$\begingroup\$ Probably can't help you there, as what I have tended to do is generate fragments of eagle xml files in everyday languages - typically C, but sometimes tools like sed for modifications. \$\endgroup\$ – Chris Stratton Aug 15 '16 at 0:57
6
\$\begingroup\$

If you are using Version 6 or later, in the device editor, use the Append button.

In the connection screen, make your connections as normal. Then if you want more than one pad in the package to be connected to the same pin in the schematic, do the following steps.

  1. Click on the connection to which you want to append a pin
  2. Click on the pad to be appended
  3. Click the append button

You should now see more than one pad name forming the connection. There is also a small symbol which looks like a trace connecting some pins (highlighted red). This indicates the type of appended connection.

If the blue line is present in the indicator, it says that they must be connected by a trace in the layout.

If you click on it, the blue line will go away. This now indicates that only one of the pins need be connected (you can connect more, but only one is needed).

In your case, you can use the latter option in a sort of "hacky" way. As you know that the pads are already electrically connected in the footprint, you can click the button to indicate that only one needs to be connected in the layout (as you know they are already connected anyway). This will remove the air wire that is annoying you.

Appending Pin

\$\endgroup\$
  • \$\begingroup\$ They were appended but I didn't know the thing in the red circle was clickable. That solved it, thanks! \$\endgroup\$ – Wesley Lee Aug 14 '16 at 22:35

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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