NRF51822 PCB layout review

RE: NRF51822 PCB layout review

ProtexFor — Tue, 25 Jul 2017 13:28:21 GMT

Hi Joseph, I read your problem, and I have also read the solutions provided by AmbystomaLabs. My idea is to do the development of a lighthouse, where you can measure the ambient temperature. No matter the size of the prototype (for now). My query is yes with your design, I will be able to get what I want. If yes, could you give me the design? On the other hand, I have to buy everything in one go. So I'm going to buy an SDK, a beacon module and 5 nRF51822 chips. I would need to know which temperature sensor I need, and what balun I'll need. If you can lend a hand to make the list of components, I also thank you. regards

RE: NRF51822 PCB layout review

joseph — Fri, 24 Feb 2017 23:45:39 GMT

Awesome, thanks for the help. I am sure that you saved me a lot of headaches had I printed my original design. Can't wait to get this thing wired up!

RE: NRF51822 PCB layout review

AmbystomaLabs — Fri, 24 Feb 2017 22:07:08 GMT

Much better! Well done. If you want you could also mirror the antenna top to bottom. (ie, rotate it about the feed point). The ground plane is a little more continuous on the top of your board.

RE: NRF51822 PCB layout review

joseph — Fri, 24 Feb 2017 21:35:15 GMT

I see what you mean. I have added the changes using the recommended balun for 51822 QFAA/QFAB on the page you sent me (2450BM14E0003).

Please have a look. http://imgur.com/a/33xSx

I have also noticed that the reference design provided by Johnson has a wider route for the antenna then I do. However, I copied the meander antenna directly from Nordic's design of the Bluetooth smart beacon. Is the current width acceptable?

Thanks!

RE: NRF51822 PCB layout review

AmbystomaLabs — Fri, 24 Feb 2017 20:14:27 GMT

The routing mistake is that the balanced pair are not the same length, are not characterized and one of them routes through on two vias using a different plane. The vias alone will really mess up the impedance. It would be preferable to put the balun right next to the chip with equal length balanced pairs and then run a characterized 50ohm line to the antenna.

RE: NRF51822 PCB layout review

joseph — Fri, 24 Feb 2017 19:45:05 GMT

The only thing I am planning on running from the chip are LEDs and 4 H-Bridges to control a few DC motors. It wont matter the voltage that the motor sit at since regulating the PWM will be the controlling mechanism.

The extra converter I am referring to would be something that gets the Lipo battery range (3.7V - 4.2V) down to a voltage that the NRF51822 can handle (3.0V - 3.3V). If I use the 51822's buck converter then I would need another buck converter or something similar to bring it down to what the 51822 can take. I might as well just have a single converter that brings the Lipo from 3.7-4.2 down to 1.8 and skip the 51822's buck converter.

I understand your argument about using the Balun chip that I did and will have that fixed. However, I am not understanding what is not appropriate about my routing. Is this because one Antenna route is going under another?

Thanks!

RE: NRF51822 PCB layout review

AmbystomaLabs — Fri, 24 Feb 2017 13:21:45 GMT

Oh, and on your updated layout you can NOT do the differential routing the way you did it. It's not appropriate at all. Plus I don't know about your experiences with WLCSP (ST balun), but I've never liked placing them and all the fab houses I work with also complain about them. This is the same balun they used on the beacon dev board. Half of the boards I received from nordic had incorrectly placed baluns. The Johanson part is a nice normal ceramic chip with leads up the sides. Placement and reflow is way easier.

RE: NRF51822 PCB layout review

AmbystomaLabs — Fri, 24 Feb 2017 13:12:38 GMT

I am not sure which extra converter you are referring to. The 51822 has an on chip buck converter that only requires an external cap and inductor. The only thing you need to do is supply the 51822 with 3.0 -3.3 and let the the 51822 do it's job. This will give you gpio at the higher vdd (3.0-3.3) which will likely help out with gpio communications with other devices. The soft device automatically controls the on chip converter and only brings it up when necessary. You could probably even make a case for running it at 2.7v. This would give you a little more operating range on the lithium battery. You just need to run all your peripherals at that same voltage what ever you choose. In case I didn't make that clear earlier, if you choose 1.8 you need to run all your peripherals at 1.8, similarly if you choose 3.0 you need to run all the peripherals at 3.0.

RE: NRF51822 PCB layout review

joseph — Fri, 24 Feb 2017 08:54:46 GMT

Hi AmbystomaLabs - I really appreciate the great comments that you have been able to provide.

I have looked at the schematic difference between the 1.8V schematic and the original schematic (the one that I am using right now) and it seems that the only difference is a single VCC line that runs to another pin on the NRF51822 which seems like an easy enough change. I read a bit about running NRF51 series from a 3.7V lipo and it seems that the Torex XC9265 PFM DC/DC switcher was recommended which I will probably end up using (ref: devzone.nordicsemi.com/.../). It seems inefficient having 2 dc/dc converters - one for the 2.1-3.6 range provided by the design ref and one for getting the Lipo within that range.

Here is a link to the latest design with balun BAL-NRF02D3 taken from Nordic's Beacon. http://imgur.com/a/5HtmY

Thanks!

RE: NRF51822 PCB layout review

AmbystomaLabs — Thu, 23 Feb 2017 13:32:57 GMT

By the way here is a link to the Johanson page of solutions for Nordic devices: www.johansontechnology.com/nordic

RE: NRF51822 PCB layout review

AmbystomaLabs — Thu, 23 Feb 2017 12:46:16 GMT

Also I should point out that by using 1.8volts for VDD you will only be able to communicate to other devices running at 1.8volts or lower. The gpio on the nRF aren't just open collector, they are all push pull. Even as an input you can't pull a gpio higher than VDD (1.8v) or the fet will reverse bias and short the VDD rail through the gpio to the device it is talking to. Also since the max signal is only 1.8v, a 3 volt device likely won't see this as a high state. Most spec 0.7VDD or for 3volts is 2.1v minimum for a high state.

If you run the nRF at 3v or 3.3v and let the on board dc/dc do it's job all these potential problems go away.

RE: NRF51822 PCB layout review

AmbystomaLabs — Thu, 23 Feb 2017 12:40:26 GMT

You could keep the matching network, but at 2.4GHz any of the trace lengths and widths will need to be precisely the same as the reference design. Differences as little as a 1mm can change the effect of the components. Also your board will likely not be made up of material with the same relative dielectric constant. Meandering lines are normally close to 50ohm by design with only a simple match. If I were choosing, I would do a chip balun to the meander and lose the complicated match. Just keep the shunt cap for the antenna.

I still think you should re-consider running the device at 1.8vdc. Unless you go through a lot of effort to make sure the ripple is low from your buck converter for the LiPo all that ripple will propagate through to the nRF. This could cause problems by modulating the RF envelope or even causing a local brown out condition causing a reset.

RE: NRF51822 PCB layout review

Roger Clark — Thu, 23 Feb 2017 03:16:52 GMT

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

RE: NRF51822 PCB layout review

joseph — Wed, 22 Feb 2017 22:25:29 GMT

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!

RE: NRF51822 PCB layout review

AmbystomaLabs — Wed, 22 Feb 2017 18:29:40 GMT

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.

RE: NRF51822 PCB layout review

joseph — Wed, 22 Feb 2017 17:51:57 GMT

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

RE: NRF51822 PCB layout review

AmbystomaLabs — Wed, 22 Feb 2017 13:39:47 GMT

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.