In Eagle PCB, how can I reuse devices from existing schematics?

I'm making an Eagle PCB schematic design, a break-out board for the TI cc2540. I have a reference Eagle design with a PCB antenna, and I would like to use that antenna.

Looking at the element "info" for this printed antenna, it appears to be in library antennas, but I can't find this library in the default Eagle libraries, nor can I find it using Google.

So my question is, where can I get this library for my BLTE chip to use a printed antenna?

Edit 1:

If this component is not available through a public library, can I select the element and "export" it so I can use in my own library?

Starting with v6, Eagle supports true copy&paste. This means that you can copy any part from one design to the windows clipboard and just paste it into another!
You can even copy/paste groups of parts, and between two different eagle instances (this wasn't possible before either).

This is a MAJOR improvement from earlier eagle versions (where the cut/copy/paste was totally counter-intuitive/horrible) and reason enough to upgrade.

Note that you have to use group select + copy even for a single party to make it work. The just paste it in any other schematic.

This way you only "import" the parts into the schematic and don't have to worry about from which library it comes or where it should go at all (assuming this is not a requirement).

The basic organization of Eagle files is that all libraries used end up in the final .brd and .sch file. There exists a User Language Program (ULP) that can export all the parts contained in a schematic, including the package footprint called exp-project-lbr.ulp. This file should be included with your Eagle installation.

(thanks to this YouTube video for the general information)

The steps are:

1. Open the schematic and board
2. Click the ULP button, or File->Run...
3. Find and run exp-project-lbr.ulp. You will be provided the dialogue below. The selected settings worked for me.
4. Click the Collect data button. You will be given another dialogue shown below. Click Yes.
5. The library containing all the parts in the schematic will be created and opened. The .lbr file will be stored in the working directory and you should be able to add it without too much difficulty to your new project.

The antenna part is ANTENNAS_TI_2.4GHZ_MIFA, but even with the layout you need to be careful that you follow the layout given, including the ground connections for it to work properly.

There is no definitive "eagle library". Generally, everyone has their own library, with the parts they have drawn up. You need to ask the people who provided the eagle files in the first place.

If they don't release the library, you'll have to draw up your own PCB trace antenna. It shouldn't be too much work, considering you have the board file, and TI has an app note specifically about that antenna.

Alternatively, it seems like it's possible to extract the parts from the eagle board file. See @W5VO's answer.

FWIW, this looks to be a project of a random hobbyist, not an official TI design:

Please note that this is not an official reference design from Texas Instruments. The board has been assembled and the functionality has been confirmed, but it has not been through RF characterization or any other forms of rigorous testing. Care should be taken when using liion batteries as these can be unstable if used improperly. Using liion cells with built-in protective circuits is highly recommended.

It looks like the wiki page for that breakout board was created by User:Kervel, who has no contact info.

• ok, I see, but would it be possible to select this element and "export it"? thanks – manuelBetancurt Sep 14 '13 at 3:37
• @MaKo - No idea. I don't use eagle. – Connor Wolf Sep 14 '13 at 3:38
• -1: if you have the pcb file, you can extract the library, as w5vo explains. – Wouter van Ooijen Sep 14 '13 at 7:22
• @WoutervanOoijen - At this point, I think W5VO's answer should be the accepted version. As I said, I'm not familiar with eagle. – Connor Wolf Sep 14 '13 at 7:53