NRF51822 PCB layout review

[joseph]

Hello,

I recently finished up the NRF51822 pcb board that I plan on getting printed. I used the reference design file provided by Nordic (NRF51x22_qfax) but added the following things:

• Meander Antenna taken from NRF51-Dongle with a bit more length added for adjustment
• Shunt Capacitor for the Meander Antenna
• Through-holes connected to most of the I/O pinouts from the chip for breakout
• Through-holes for power in (1.8V & GND)
• Increase in GND plate size with vias to match

I am rather new at working with the NRF51 series as well as PCB design. Any advice would be great help. I am mostly concerned over the way my antenna is structured and if a single shunt cap should be enough for this.

Thanks!

Image of Front

Image of Back

Altium PcbDoc Source File

[AmbystomaLabs]

I just took a look at the jpeg's you sent out and not the Altium file. It looks like you are making a development styled board.

I would suggest you implement both the dc/dc for up to 3.6vdc and a 1.8 vdc low voltage connection. It seems like more people are likely to run it on 3.3 from other sources than a 1.8vdc source. This way they could do either.

The balun/matching for your meander is kind of messy. There are several good chip style LC baluns with match and harmonic filtering for the 51822. They will take up less board space and give you an easier RF solution. One is made by Johanson.

You should put more capacitance local to the 51822. It looks like you are using the bare minimum from the reference design and you may have lost some of the bypass caps. Processors need quite a bit of instantaneous current to operate and local caps provide this. Also, if the device is run on a coin cell these have very high internal resistance and the losses could put you locally into a brown out state during a Tx burst.

The footprint for the 51822 seems ok, but I didn't measure it. Looks like a nice via grid.

You broke the ground plane to run power from the left side to the right side. The clock lines will radiate more this way and you will probably introduce some clock noise and harmonics into the nearby gpio/adc connections. At least you did this at right angles, but it could give you some headaches.

Connections 19 and 20 are kind of in the middle of nowhere and will couple a little with the meander. If it was me, I would figure out a way to move the connections around so they are all back behind the ground plane.

If it's meant to be a development board that someone may permanently mount inside a product, you should put some unplated mounting holes on the board. This will make mounting a lot easier than drilling holes.

[joseph]

Thanks for the comment!

I am planning to run this off of a 3.7v Lipo battery that will have an external circuit to regulate it down to 1.8v-2.1v. The DC/DC is not enough to handle the up to 4.2V that the battery could provide and I don't need the power saving that comes from the 1.8v only circuit.

I copied the NRF51x22_qfac reference design completely and did not lose any caps in the processes. I thought that the reference design had just enough components to get it working properly. Are you recommending that I add some new bypass caps not shown on the original circuit. Do you have a link to such a design?

I can't quite pinpoint where I broke the GND plate. Is it the fragment that the GND throughhole is connected to since it only has a single via?

I want to keep a PCB antenna rather then a chip. Do you have any recommendations on how I could fix my current one?

Thanks! Joseph

[AmbystomaLabs]

The break in the ground plane is visible on the ground plane layer. You ran VDD from the left side to the right side under the gpio and 32MHz clock. This forces the ground current to travel around the break which will introduce more noise. Also, clock and harmonics will propagate through the vdd line and ground break and make it's way onto your gpio. This would only be a problem though if you use them as ADC.

I did not refer to a chip antenna. I referred to a chip balun. The 51822 has a balanced RF connection the external discretes do the balanced to unbalanced (ie, single ended) conversion and matching. There are good chip solutions for baluns that take up a fraction of the space, are predictable and also include harmonic filtering.

[joseph]

Thanks for the reply. I have fixed all of the issues you mentioned except for the antenna which I am still not too sure about.

I have read here (devzone.nordicsemi.com/.../) where it talks about how the NRF51-DK simply has a shunt capacitor for its PCB antenna. They mention in the comment section that the matching network included in the reference file, up to and including C6, could be replaced with a Balun. However, I want to keep the current matching network and just add that shunt capacitor. Shouldn't that be fine?

Thanks!

[Roger Clark]

I'd also be concerned that pins 19 and 20 are probably too close to the antenna and may effect the field pattern and range etc