PCB design for STM32WB55CE Bluetooth MCU

Thread Starter


Joined Jul 21, 2020
I designed a pcb around the STM32WB55CE. The RF design is meant for the capabilities needed for 2.4GHz bluetooth. I looked at the available AN's and did my first shot with the design. Please keep in mind, that this is my first RF circuitry.
For the RF matching, I chose the IC provided by STM. As an antenna I thought I'd go with a ceramic one, because I want the pcb to be small and also reliable (as opposed to a pcb antenna).

For the PCB itself, it's a 4 layer stackup (see the attached pictures) with:
top layer(red) -> signals only
inner layer 1(yellow) -> ground plane
inner layer 2(orange) -> power plane
bottom layer(blue) -> ground + signaling

The area around the antenna that is suggested to be kept free of metal is the silkscreen on the pcb pictures. I made the metal free area a bit bigger though, just to be on the safe side.
I also read about via fencing, but wasn't sure if it's a hard neccesity.
In general the bluetooth should work only within 2-3 metres.

The signals that are broken out are all digital with 3 exceptions. PA10, PA11, and PA12 will be used for analog readings .

Any suggestions are appreciated :)




Joined Jan 19, 2021
8dm7bz, I haven't done RF in some time, but I'm guessing you will need controlled impedance and your board vendor can help with that. This will be 50 ohms for sure and that said, the 4 layer stackup is a bad idea unless done right, Your stackup shows the dielectric is thicker between L2 and L3 so you don't get much decoupling for power with that configuration and return paths for signals get mixed with power and generially will cause more issues that you want. . If you can, I would suggest using L2 and L3 as Ground/Returns and route your power on the surface layers. You will need to get your vendor to give you a trace width and that's based on the dielectric thickness between L1 and L2. That needs to be controlled along with the trace width since it is that relationship along with the Dk of the board materials being used. Flood the top with 3.3V to get power de-coupling with Ground. Having GND on both inside layers, this gives you a better return path for all the signals since Ground is under every signal. You should also add several ground vias in the board to tie the inner planes better, (1 via per sq in.) As far as via walls go, you may not need them on this layout since it is a very short run to the antenna board and if you're not calling out a controlled impedance, you may not get the expected results with the vias? That said, in this case, I would review the antenna datasheet and their reference board for the way to flood the surface layer of the board with Ground.
Some things I noticed on your layout.
1. Top side you have several chip components, (3.3V decoupling caps) on the left side that are grounded with a long string connected to 1 via. You should ground each component with it's own via. The inductance of that long trace to the ground via is not going to help at high frequencies. If you want, add a copper pour along that side and add a GND via between each chip, that's better than what you have if you can't put a via at each chip.
2. In addition to the long GND path, your OSC, (Y1). device should be grounded as close as possible to the part and the same goes for the power to it. Long lines like these are or can be EMI issues and possibly cause instability of the circuit. The EN line can be small but GND traces should be fat and short. (That goes for all Power and Ground traces when ever possible.)
3. I notice the trace from pin 21, (RF-IN) is wider and continues out from the Filter that way also, are you controlling the output impedance here to 50 ohms? Like I said, if you are calling out controlled impedance, the 4 layer stackup you have is not a good choice in my opinion. That said, the GND via to the filter has a small trace and should be wider. In fact, filters like that should have a via on the top and bottom near the input and output and as close to the filter as you can get. Look at Fig 13 of that filter data sheet, they show a good way to provide the ground area for that part. Flooding the area around the filter as they show is good and the vias are symmetrical on both sides of the output to control the return fields. I suspect you used their stackup for your design which is something I/we take with a grain of salt. The manufacture can create layouts and stackups for their parts, but that's not always the case in the real world. :)
4. The antenna connections have a small trace to the GND pins and they are daisy chained like the caps I mentioned above. I noticed how the manufacture used a reference board for testing and that board is likely never what you will need in the real world. If you look at their data sheet, you can see how they used a matching network, which you may not need because of the filter, but I believe you need ground copper up to the top of the board and just keep it away by about half the width of the antenna all around. You can do that on all the layers which will allow you to have ground all the way up in that area, The only thing I'm not sure about is copper under the antenna on the inner layers. That's why I said keep is away by half the width. They do show a smaller trace running to the antenna but it is most likely very short, like less than 1/2 wavelength before becoming part of the flooded ground area. You should have vias stitched around that area and they should be along the flooded area edge. (Via wall you mentioned) Don't share vias to pads in RF, those engineers really don't like that. :)
5. I like the way you flooded L4 with GND but if you put GND on the inner layers, that L4 flood could be 3.3V and provide more power coupling.
That's all I can offer for now and there may be more but I didn't get a lot of time to review more. Hope this helps a little? Your routing and placement looks good. so you are heading in the right direction.

Thread Starter


Joined Jul 21, 2020
Thank you very much. Just a couple days later I found a nifty little chip by STM called STM32WB5MMG. I'm going forward with that one since, it's smaller and probably performs better than anything I could come up with.

But I will come back to your list of recommendations for future designs :)