I am working on a BLE Gamepad project using a module based on the Nordic NRF51822. This is the first project I have done that is more complicated then an arduino project so I am likely to make some big mistakes. I am getting close to finishing it, but I have this aching feeling like I am doing the power rails completely wrong.

I currently have one long +3V3 trace running under all the circuitry that powers two LED's, two analog thumbsticks, and the microcontroller module. In a four layer board I would have separate traces for AVDD and VDD, but I am already beginning to feel a little cramped in the areas where power traces are needed. I might be able to separate them if I route VDD under the module itself, but I am worried that it might cause noise in the module if I do this. Essentially, I would like to know what I should do for power routing in such an environment.

For specifics check out the github project with pics, gerbers, and the source for the KiCad project files.

If you see things that are wrong with the design and are not related to this question then feel free to post about them at this reddit post

  • \$\begingroup\$ I took a quick look at your files. The one thing I suggest that you should do is to scatter vias on the ground planes such that the top and bottom planes are stitched together especially across areas cut by traces. It is easy and can only help. The VDD is probably fine the way it is. Although I may be tempted to just run that through the middle to minimize the total length to everything (with the ground stitched accordingly), it is hard to say from just glancing at the images. \$\endgroup\$
    – rioraxe
    Apr 23, 2016 at 5:13

1 Answer 1


I haven't looked at your files. ...In general, for a two layer board I would put the bottom layer to be a ground plane and keep the power delivery traces short and wide on the top layer. There will no doubt be places that the signals will need to cross, and it's fine to take them on to layer 2 but be careful not to make any copper Islands and not to break any continuous ground underneath the power delivery.

It is almost certain that you need to keep the copper away from the bluetooth module because it will mess with the antennae. Are there any impedance controlled nets in your design? If so this might be more difficult on a 2 layer board

Okay I have had a look at the png images on your github page and its not clear what you are asking. I can see 2 traces under the module: pin 38 bt_led and pin 28 select. Both of these can easily be moved onto L2 and I would suggest stitching vias on either side.

Your biggest problem is the chunk of signals on the right hand side passing directly underneath U2 and L4. These will pick up huge amounts of noise from the switcher. They must be routed somewhere else or move the psu to be above a ground plane

As for your specific question, the avdd is already separated from the rest because you have them joined at the smps output. D1 is the only thing that also uses this trace, but I don't imagine it will be particularly fast. So not a problem as it is. You should definitely decouple the other supply to the module at pin 14, and possibly add some lower value ceramics alongside c1. 10n perhaps

  • \$\begingroup\$ From a quick google search, I would say I don't have impedance controlled nets, but I don't know much about the subject. I am mostly concerned about getting an answer to "Is it okay to route power rails on the power plane under the module with the microcontroller?" In either case it would probably be best to consider the specific example which can be seen in my files because I actually had to put components on both sides of the board. \$\endgroup\$
    – Nate
    Apr 22, 2016 at 22:43
  • \$\begingroup\$ Added some detail based on your comment. Impedance control is for things like usb, sata, antennae. Generally fast signaling You don't have any thing like that. \$\endgroup\$
    – Loganf
    Apr 23, 2016 at 9:59
  • \$\begingroup\$ My original post was referring to the intended design not the current one. I want to separate the digital power traces for the module and LED's from the analog power traces that are connected to JS_L1 and JS_R1 by running the digital power rail along the top underneath the module. You have a point about U2/L4. I just don't really know what I can do about it. I might be able to remove the screw at P4 and put it there, but that is really the only option that doesn't interfere with some signal. Still I suppose I can do better than what I have now. \$\endgroup\$
    – Nate
    Apr 25, 2016 at 19:36
  • \$\begingroup\$ I apparently don't know enough about when, where, and what value of decoupling capacitors are needed. I'll try researching this on my own but I would appreciate links if you have some. \$\endgroup\$
    – Nate
    Apr 25, 2016 at 19:43

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.