Problems creating an PCB track NFC antenna

Question

I'm trying to create a PCB track NFC antenna as an Eagle part. As part of this I need a via so I can bring out the connection from the centre of the coil. Is it possible in a library part?

Also, the antenna involves a trace which appears to "short" two nets, so I get an overlap DRC error. Is it possible to avoid this?

I took a look at Sparkfun's RFID evaluation shield to see if that gave me any clues. They apparently went for the antenna as part of the design rather than a library part (avoiding the via issue) but still appear to have similar overlap errors.

https://www.sparkfun.com/products/10406

berniwa · Accepted Answer

Hey David, it is much simpler if you do the antenna in the board and not in the library, as you can do a design without the mentioned DRC errors. It basically just: 1. Short the pins out in schematics. 2. Draw the antenna wires as suggested in the design note of the NFC IC. A few tips when working with NFC: In order for the antenna to work properly you'll need to individually match to your antenna, and in most cases you won't get away with the matching from another design. So make sure, to have a least two footprints (0805, 0603 or 0402) for each matching component, this will allow you to solder capacitors in parallel what allows you to to trial and error test matching easier. Greets Berni

geralds · Answer

Hi David,

For more information how to design an PCB printed antenna you can find it here, for example:

https://www.autodesk.com/products/eagle/blog/rfid-works-antenna-design/

Here you'll find a reference design:

http://www.st.com/content/ccc/resource/technical/document/application_note/d9/29/ad/cc/04/7c/4c/1e/CD00221490.pdf/files/…

Here there are some chip manufacturer they makes RFID chips and also have their reference designs.

www.ti.com

www.maximintegrated.com

www.microchip.com

www.atmel.com (microchip)

www.silabs.com

www.cypress.com

In the Eagle you can make PCB printed coils with the print-inductor.ulp

Just click in the PCB on the menu item "tools" and "calculate printed-coils", then a menu window pops up with that you can create your printed inductor.

--

Or there is also the ulp - spiral-coil.ulp what you can use for.

Click in the PCB on the button ULP: select the file spiral-coil.ulp

(this is a bit older and smaller ulp file but it works fine)

As suggested, yes, you also needs parts for the impedance correction.

Best Regards,

Gerald

---

Problems creating an PCB track NFC antenna

Top Replies