Chip Antenna Pi Network Circuit Layout

[parthjain]

Hi there!

I'm looking to layout a chip antenna using the nRF52832 WLCSP chip and am confused about the layout of the antenna matching circuit. The reference design (CIAA) provided by Nordic has a layout with one cap, one inductor and a PCB antenna. I have read that this design should be copied exactly, however, the chip antenna spec shows a different layout for the matching circuit. I am not sure which layout to follow.

I understand that since I am using a chip antenna, I am better off with a 3-component pi matching network. Should I simply add another capacitor to the CIAA reference design from Nordic? Ideally I would place my network close to the ANT pin of the nRF but not in the exact layout to save space, since it is a board limited design.

The antenna I am using is: AF 216M245001

Any help is appreciated, Parth

[AmbystomaLabs]

All antennae have different matching requirements. A Pi network is sort of the RF equivalent of everything but the kitchen sink. The Pi network gives you 2 shunts and one series component which can normally solve the worst of matching disasters.

On the reference designs, the PCB antennae generally have simple matching needs that Nordic has painstakingly reduced to the fewest components.

However, your chip antenna even if you do a really good job of following the manafacturers layout guidelines may not have a simple match. Therefore it is better to put spots for 3 components (ie, Pi) vs just a single shunt or something else.

You will have to determine which components and values are required by actually matching your antenna after you spin your board. Generally, if some of the Pi is unused it is better to leave well enough alone and do not change the layout. You would likely change the match by changing the layout.

1. So do the layout per the antennae manufacturers spec.
2. Place a Pi network in the 50ohm feed to the antenna where there is a stable ground plane. Normally this is close to the nRF.
3. Spin the board
4. Figure out the match for the antenna.

[parthjain]

Thanks for the response! You mention the 3-component Pi network can solve most antenna matching scenarios. If I layout the matching network differently than the reference design, and tune it after spinning out the board would I see an issue? I plan on routing all of the Pi network components on a stable ground and close to the nRF, except in a different orientation than the reference design, plus the additional shunt capacitor.

[FormerMember]

The matching network in the reference layout matches the chip to 50 Ohm. In addition, a pi-network is needed to match the antenna to 50 Ohm. The tutorial "General PCB design guidelines for nRF52" explains more on this topic.

[AmbystomaLabs]

Functionally you can put the pi network anywhere along the 50ohm feed between the nRF and the edge of the ground plane just before it goes to the antenna. In practice you will want to keep this 50ohm feed as short as possible due to board losses. Invariably this results in the pi network being close to the nRF.

As Kristin pointed out, the shunt C series L at the output of the nRF need to be placed right next to the nRF as per the product spec. If you were to move these they would no longer match the nRF correctly. The Pi network is then placed after the nRF match.

In practice it is trivial to combine the nRF match and antenna match into one 2 or 3 component match. But for your efforts I would advise against it and just copy the nRF match over to your board. Make sure you model your 50ohm microstrip correctly. For an 0.062" board the best approach is a coplanar waveguide with ground.

[parthjain]

Okay understood. I was confused that the Pi network and the nRF matching network were one in the same. So in total my matching for both the nRF and antenna would be 5 components to be as safe as possible. A 2-component matching for the nRF and a 3-component Pi network following it to match the antenna.