3
\$\begingroup\$

I'm designing a board that should contain an antenna I found in an application note. I'm using Eagle and I tried to create a library part for the antenna. However, since the antenna is basically a fancy-shaped short circuit, Eagle tends to report DRC error for it.

Is there a way to draw a PCB antenna in Eagle in such a way, that the DRC errors wouldn't show up?

Antenna with DRC errors

\$\endgroup\$
  • \$\begingroup\$ Please use SEs image uploader to post your image. As it is now it takes a few seconds to load for me. Also we want to make sure images stay with the question for the long term. \$\endgroup\$ – Kellenjb Dec 29 '11 at 18:52
  • \$\begingroup\$ Hi is there anywhere i can download that component? I have been looking for a pre made one.. for ti253x \$\endgroup\$ – Piotr Kula Feb 10 '12 at 9:21
  • 1
    \$\begingroup\$ @ppumkin, sure, grab it here: technika.junior.cz/trac/browser/eagle_libraries/… \$\endgroup\$ – avakar Feb 11 '12 at 13:08
5
\$\begingroup\$

No, there is not. Well, not for an antenna- You can make a junction with a soldermask opening that will create a short (if you use a stencil cut from the output of the CAM tools), but there's no way to join two different nets on a copper layer in the PCB editor.

Just keep doing what you're doing; it will produce a DRC error but that's OK.

As I wrote at How do I facilitate keeping multiple grounds, (i.e. AGND, DGND, etc…) separated in the layout when using Eagle?, you can move on by select one of the errors to enable the "Processed" and "Approve" buttons ("Approve" is the only one I use on a regular basis) and choosing "Approve" to move the error from the errors list to the approved list:

Error moved to approved list in errors dialog

and will stay there on subsequent runs of the DRC. Note that this only moves this specific error with this specific pair of nets at this specific location. Closing this window and running the DRC again produces the notification "DRC: 1 approved errors"

DRC: 1 approved errors

and no "DRC Errors" dialog. When you don't get a new DRC errors dialog, you're done!

\$\endgroup\$
2
\$\begingroup\$

As of Eagle version 5 at least, no it is not possible. You can make a library part with arbitrary fancy copper shapes, but you will get DRC errors. You only have to go thru the DRC errors once and approve them, then they won't pop up again unless you touch that part.

I hear that there will be a way someday to define arbitrary pad shapes in a library part and have DRC not complain. That may already be available in the new version 6, but I'm not going near that for a while so I wouldn't know. Let all the people who don't have better things to do find the bugs in the major new version of Eagle.

\$\endgroup\$
  • \$\begingroup\$ It's hard to read in the Aero semi-transparent menu bar, but it looks like the OP is using Eagle 5.11 Light. \$\endgroup\$ – Kevin Vermeer Dec 29 '11 at 19:03
  • \$\begingroup\$ @KevinVermeer, that's correct, I haven't had time to check out Eagle 6 either :) \$\endgroup\$ – avakar Dec 29 '11 at 19:55
  • \$\begingroup\$ @avakar,Eagle 6 gets rid of the overlap and clearance warnings, but I still get a warning for width because it seems to look at the width of the wire (0 in my case) instead of the width of the polygon \$\endgroup\$ – John La Rooy Jan 16 '12 at 6:09

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.