I realize there are some questions that are related to this topic but I didn't see any that are really RF specific.

I am working on a 2-layer Bluetooth module and I have some unused spaces on the top layer that I can't decide if they should be ground pours with stitching vias to the bottom layer (which is primarily a solid ground plane) or not. I've been doing a lot of reading/research and there seems to be conflicting ideas about top layer ground pours. So, I'm reaching out to you folks and hoping that someone with experience in this (RF board design is a plus) can shed some light on this topic for me.


For anyone else looking into this or are just interested here are some good resources that I've found helpful:

  1. http://www.maximintegrated.com/en/app-notes/index.mvp/id/5100#10
  2. http://www.eeweb.com/blog/circuit_projects/basic-concepts-of-designing-an-rf-pcb-board
  3. http://www.eetimes.com/document.asp?doc_id=1279446
  4. http://www.atmel.com/images/atmel-42131-rf-layout-with-microstrip_application-note_at02865.pdf
  5. http://www.icd.com.au/articles/Copper_Ground_Pours_AN2010_4.pdf
  6. http://www.ti.com/general/docs/lit/getliterature.tsp?literatureNumber=swra367a&fileType=pdf

Most of the sources above mention ground pours, and overall RF design.

  • 1
    \$\begingroup\$ One thing you might have to worry about is capacitative coupling between top pour and your RF traces--be careful that the spacing in the design rules is at least twice your trace width. Also, I believe Olin has gone on record saying a top ground pour doesn't make a difference in a 2-layer board but I can't find the post now. \$\endgroup\$
    – Paul L
    Jun 2, 2015 at 2:59
  • 3
    \$\begingroup\$ Here's his post: electronics.stackexchange.com/a/41923/56232 \$\endgroup\$
    – Paul L
    Jun 2, 2015 at 3:04

1 Answer 1


RF Engineering is "Pure Black Magic." Proponents will insist it is not, but unless you have a PhD in physics, it probably will seem so. The concepts of resistance, capacitance, and inductance, which makes sense at DC and low-frequency (up to some MHz), are completely skewed when it comes to high-frequency design and implementation. Traces can behave more like resistors or impedance elements, pads and gaps seem like capacitors, corners like reflectors, etc. The full complexities are beyond even a short book on the topic.

The short answer is, "RF" and "2-sided PCB" are seldom heard of together. Most RF (transmitting) devices use a 4 or more layer PCB, and the outside layers are typically ground planes. Some will say this is more to err on the side of caution, but for someone unfamiliar with RF design, it can mean the difference between a working design or not.

For a transceiver device like Bluetooth, near the location of the antenna when transmitting, the electromagnetic field produced can couple to nearby traces (especially as their length approaches a quarter of the wavelength) and induce voltages and currents, causing erratic behavior. That is why ground planes are used; to absorb these waves. Near the antenna the EM is strongest, so they can't be laid arbitrarily there; dimensions and even shape can be critical for correct operation. Further away, it becomes less of an issue, as the EM field dissipates at the inverse square of distance. This TI app note touches on some of the other details at high frequencies.

I'd say the most practical solution is to find a reference PCB layout for the particular BT device being utilized and start from there. Hopefully the manufacturer has made one available. For comparison's sake, here is a small picture of one such design. It's datasheet doesn't mention much about the PCB, likely because the designer spent a great deal of time working on it. The PCB appears as though it could be a 2-sided one, however this is unclear. A larger photo can be seen here. Traces are seen on the top side and you may be thinking "Aaha! I knew 2-sided could be done..." however some tiny but very important things are noticeable:

  • There are a strip of vias below the antenna. These are closely-spaced to short out all of the strongest EM field to ground.

  • It's impossible to tell if the left side of the antenna shorts to ground under the silkscreen logo. If it does, it may be a PIFA antenna.

  • There is definitely at least a partial ground plane on the reverse side, as the majority of the center PCB is dark. As Olin explains in Paul's link above, a few small pads and traces here and there probably won't matter much, but an inch-long trace or group of non-grounded-anywhere-parts is asking for trouble.

  • The micro-vias seen in some of the front-side traces likely connect to the ground plane. These were not placed willy-nilly, but fill in as much of the top surface as possible to reduce EMI there the best it can. (This is an attempt at trying to produce a robust device without using more layers.) It may be that there are enough top ground areas, covering enough of the surface, that it prevents much coupling there. (Ever wonder why a microwave oven has holes in the door, but no microwaves come through? That's because the holes are much smaller than the frequency (wavelength), so the microwaves cannot penetrate it.)

  • There are likely traces on the back side underneath the antenna which seem to "do nothing" or connect nowhere. Like squares or rectangles. This is where the really funny business of RF comes into play. Remember at high frequencies, a pad can appear as a capacitor. So those traces are probably designed to introduce some capacitance or coupling physically at that location, even through the PCB. This can be done to "connect" one part of a resonating element (antenna) with another, even though no physical connection exists.

  • \$\begingroup\$ Thanks for the lengthy and detailed answer. I appreciate your help and time. I have looked at other reference designs as well and they all seem to have islands of ground pours on the top layer. It's my understanding that some of these may be acting as a shield from outside EMI and RF interference. I have pretty much copied a reference design but my board has to be a little different because of the interconnect and an additional IC, which changes the layout enough to where I have some empty spaces. I don't think it can hurt filling them in if I stitch them well? \$\endgroup\$ Jun 2, 2015 at 18:03
  • \$\begingroup\$ It looks like to me that the reference designs that I've looked at would have more ground pours on the top side if space allowed for them (most of the modules breakout to the edges of the board). This will be my second version, as I made a major mistake on my first. So this time around I am being very picky. RF design is like magic. It's amazing how a small change or something you wouldn't think would cause a problem does. Not to mention some of the crazy antenna designs. Anyone have Merlin's contact info? \$\endgroup\$ Jun 2, 2015 at 18:07
  • \$\begingroup\$ I'd say, design it for alteration and plan on a revision or two. Leave some ground pads un-masked, and if it doesn't work, try soldering a little metal shield over that part. If a signal line is suspected of picking up EMI, scrape off some insulation and solder a 20pF cap or whatnot across it. And look into ferrite beads, they are lossy at certain frequencies but their inductance can be tricky. Unfortunately for us mortals, Merlin's phone number is +x-xxx-xxx-xxxx. (Wouldn't let me use $ symbols, ha!) \$\endgroup\$
    – rdtsc
    Jun 2, 2015 at 18:22
  • \$\begingroup\$ Thanks again! Sounds like a plan. I'm just going to go with what I've learned and make the best judgement I can about ground pours on the top. LOL, good link to "Merlin". \$\endgroup\$ Jun 2, 2015 at 19:09

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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