Ground Planes and BLE Performance

I have a product using a Nordic-based Laird BLE module with PBC trace antenna and RF power amp that puts out +18dBm. The Laird dev board gives 300ft+ range, but the product, with a fairly small 60x60mm PCB, only gets 100ft or so in the target application (which involves highly sub-optimal transceiver placement). I figure the discrepancy is likely due to my much smaller ground plane area, as the dev kit PCB is around 175 x 100mm. But another difference is that the dev board has external copper flood areas that are stitched (presumably) to at least one internal ground plane with many vias, whereas my board has one continuous inner ground plane layer and no external floods.

My question to the RF gurus here like @jpnorair is whether the performance of my board might be improved by adding outer layer ground floods with stitching. My understanding is that only area is important, but I’ve been wrong before :slight_smile:


Pictures would be be a big help if you can provide them.

What type of Bluetooth antenna (all PCB antennas are traces - tell me more) are you using?

Is your unit mounted in something, or is it laying on the desk? Pictures of the test environment would be helpful. Similarly, in the eval board mounted?

You can probably fake the ground effects with copper tape. I’m reluctant to say your inner layer ground plane isn’t a significant difference. I don’t think it should be, but it certainly could be as a result of of other factors.

100 vs 300 ft translates to about 10 dB difference in signal. Were it me, I’d be testing the antenna separately with a connector or pigtail to the board, but I’m guessing you don’t have the toys or background for that based on your request. Does the eval board have an antenna connector option?


1 Like

I echo @rich’s comments and questions. To see how ground plane and enclosure can affect something similar to your general description, section 5.1 of might show you how either the reflection is increased in general or your centre frequency is shifted away and at your band the antenna is no longer as efficient. If you can spare the modules, you could destructively test by incrementally shortening the elements (depending on the trace design you have) and seeing if/which way performance changes. Also, definitely try adding metal like the copper tape rich suggested in proximity. Perhaps before you start slicing!

Here’s the Laird BL654PA module with its PCB antenna:


Here it is on my board

and here it is in its enclosure

@smerrett79 that’s an informative app note, thanks, but this project is about using an off-the-shelf module with onboard antenna. These guys don’t have enough money to pay me to fiddle with antenna tuning, let alone someone who actually knows what they’re doing. They chose the module, they chose the product’s form factor, and for various reasons an external antenna is not viable. I guess I’ll just try the copper floods on the next spin and see if it picks up any range.

In the final application, the plastic-enclosed transceiver goes (I kid you not) into a metal box. It is what it is. But the dev board did give acceptable range from inside said box.

Being scared of everything which is RF I would rule out any power supply issue and be sure the module is able and it is trying to transmit at full power …maybe you have already done that…

Don’t you need to have a cutout in the main PCB below the area of the module with the antenna?

1 Like

That’s what I thought but if you look at the datasheet @kvk Julia is following as well as she can. Blue arrow shows copper is following keep out guidelines

Shows the keep out area and grounding pads (which I was initially worried about on the picture (in red)

@JuliaTruchsess I’m the master of wild goose chases but this is what’s on my mind.

Datasheet says dev board uses 1mm PCB thickness. And “A different host PCB thickness dielectric will have small effect on antenna.”. Is this something you have done / could do on next spin?

“Minimum safe distance for metals without seriously compromising the antenna (tuning) is 40 mm top/bottom and 30 mm
left or right.” Well obviously that’s not possible in your 60 x 60mm envelope but with the dev kit can you get the antenna into the exact position within the enclosure that yours would be and measure the range distance (perhaps on lower power setting so you don’t need to walk so far!) change as you vary its proximity to the edge? Then maybe you can see whether pulling your PCB back by even a few mm might make any improvement.

Do you have board mounting hardware in proximity to the module? It doesn’t look like it but worth thinking about.

Are you confident that the soldering under the pads connected to the vias in the red circle (and those under the module along the edge of the antenna) is good? If those pads have not been connected, perhaps the ground plane is messed up at a critical place wrt to the antenna.

I have been using the Esp32 and in that one no PCB is allowed below the module antenna part. It seems in the layout it’s a keep out area, and the FR4 will still influence the antenna properties

Laird specify it differently to esp32 and have tuned their antenna for the presence of PCB underneath:

The BL654PA development board was used for BL654PA development and the 453-00020 PCB antenna performance
evaluation. To obtain similar performance, follow guidelines in section PCB Layout on Host PCB for the 453-00020 to allow the
on-board PCB antenna to radiate and reduce proximity effects due to nearby host PCB GND copper or metal covers.

The BL654PA development board has the 453-00020 module on the edge of the board (not in the corner). The antenna
keep-out area is defined by the BL654PA development board which was used for module development and antenna
performance evaluation is shown in Figure 9, where the antenna keep-out area is ~5 mm wide, ~39.95 mm long; with PCB
dielectric (no copper) height ~1 mm sitting under the 453-00020 PCB trace antenna.
:black_small_square: The 453-00020 PCB trace antenna is tuned when the 453-00020 is sitting on development board (host PCB) with size of
132 mm x 85 mm x 1mm.
:black_small_square: A different host PCB thickness dielectric will have small effect on antennThe BL654PA development board was used for BL654PA development and the 453-00020 PCB antenna performance
evaluation. To obtain similar performance, follow guidelines in section PCB Layout on Host PCB for the 453-00020 to allow the
on-board PCB antenna to radiate and reduce proximity effects due to nearby host PCB GND copper or metal covers.

I’m 95% sure that the dev board is actually 1.5 - 1.6mm, but I’ll check if and when it ever stops snowing so I can get to the shop :slight_smile:

There are screws at the corners of the enclosure; we could try plastic screws, but with all the metal around in the final application it seems a bit pointless.

This module is a pain to solder, with small pads all underneath, so it’s not really possible to check my in-house reflow. I’m urging the client to have a dozen boards assembled outside in order to remove this variable.

Interesting. If this is the case I’d be tempted to try and get a Laird FAE to comment. They should expect to have to explain this if they are so particular about it in their current datasheet. In fact, perhaps you could see if they have any other canons about the ground-plane / keepout / dielectric/stack etc.

Well at least that’s a variable you can change in isolation and relatively quickly (before a respun PCB). If there is a screw in line with the keep-out area, perhaps a few more non-metallic millimetres before the inner surface of the enclosure could help.

It certainly looks like it. I don’t think this is worth worrying about too much but sometimes you want to look under every rock so I thought I’d mention it.

Is there any chance to move the PCB edge away from the enclosure surface at all on that side? Did the dev board go in that exact enclosure or a larger metal one, when you tested it in situ?

If the antenna is being detuned to a different band, rather than wholesale attenuated and there is no better performance than in the band you are in, removing PCB substrate may be a possibility for compensating. But it sounds like this project doesn’t have the budget for trying this out.

I don’t know whether the NRF tools allow you to select specific channels. If so, would you be able to test if the range performance at max, min and mid band channels is different? This may allow you to do a coarse approximation of the antenna sensitivity (assuming rf power output remains the same across all channels). You could then perhaps equate better performance in the lowest frequency channel as an indication of down tuning the antenna. Then PCB removal in the keepout zone might be a way to tune it back up (dremel, test, dremel, test…).

Thanks for the photos, context is helpful.

Before I did anything, I’d do range checks at several different bearings. See discussion on antennas and multipath towards the end.

Without being able to poke at it , all I can offer is a shot in the dark based on no particular insight: I don’t know if you have a sacrificial unit, but you might try cutting the PCB out from under the module antenna section.

Were both boards physically mounted the same way when doing the A/B comparison? Mounting can make a big difference in stray radiation and this can help or hurt. If the whole board is flapping at 2.45 GHz…

Maybe not a factor in this case, but with RF, ground never is. If you have two planes, the only way to get them close to each other is with generous via stitching. I’d try it in the next rev and make it a habit with RF. The higher the frequency, the closer the vias. As a thumbrule you want stitching WAY under a tenth of a wavelength. At 2.5 GHz this is1.2 CM, BUT the dielectric constant of the board makes a wavelength in board about 60% of this or 0.72 CM, but call it 5 mm. And this is just a thumbrule. For stuff like coplanar waveguide or low impedance RF stuff like PA output circuitry, lots more is better.

Another issue is that we tend to think of these radios as having a spherical wave front - equally good (or poor) in all directions. Reality usually departs from this in substantial ways. Antenna patterns are generally messy, with peaks and deep (20+ dB) nulls. A lot of engineering effort is applied to controlling patterns. I would not be at all surprised to see dramatically different ranges on your range measurements on slightly different bearings. At these frequencies reflections are a major concern. The environment is a lot like looking at a flashlight in a hall of mirrors. This is the big reason the stuff works reasonably well in spite of poor antennas. And that reflection environment (RF Systems types call this multipath) changes in real time. Does your unit have a cooling fan? It’s a moving reflector. Plastic blades - moving dielectric (think lens) still causes changes. Some one walking by - looks like a sequined Vegas showgirl to BT.

What you describe is common. The only reason this works at all is the multiple paths caused by reflections. It’s likely the metal box is pretty leaky at 2.45 GHz unless a lot of effort was taken to make it RF tight. I’m betting no effort was taken. Still, it’s going to have some impact, and it’s mostly going to be negative.


Yes, customer tries various azimuths and antenna orientations when testing range.

I wasn’t present, but AFAIK they just put the bare dev board (maybe in bubblewrap or something) into the metal enclosure, similarly to how the final board would go.

Yes, I’m aware, thanks. Obviously there’s no stitching with only one internal plane. If I add planes I will stitch the heck out of them. But the original question “Are additional planes likely to help?” hasn’t really been answered :slight_smile:

Yes, we are aware and have seen it in testing.

Nope, nothing moving during operation, and final environment is outdoors and generally far from humans (apart from the operator).

Yes, mercifully it’s very leaky, otherwise it wouldn’t work at all, as I was discussing with Mike Faraday just the other day :smiley:

OK, so much for me being “sure”, lol. It is in fact 1mm, which is good news because it means a bit of hope that range will improve if I go to 1mm. Thanks @smerrett79 for bringing it up.

1 Like

At least you left yourself 5% get-out!

I don’t know what stackup your current board is on but maybe that extra Z height between the plane of your antenna trace and the ground plane it is supposed to be working with is an issue. Says the module PCB is 0.6mm thick:

So if you are using 0.2 or 0.1mm prepreg maybe this changes things but it does seem rather fussy if this is the critical parameter (as in, their integration section should talk about whether ground plane has to be surface pour etc).

Just because I wanted to know, I checked what it would look like for the antenna proximity to vary between the surface copper pour and both 0.1mm and 0.2mm prepreg (the blue - 0.1mm and orange - 0.2mm coloured layers below the module). Using the module pads as a reference to the edge of the PCB antenna trace, it doesn’t look significant to me. Still worth talking to an FAE, though, not me!

Who is writing the test fw for this? I still would try and get them to test range on different channels. Or RSSI if available, to save the walking! Also, how is the client’s test ensuring no sigificant variation in the electromagnetic environment between tests of the custom vs dev board?

Sorry, thought I had but see that I had not.

The answer is so unlikely to make a difference as to not be observable.

I suspect the most likely difference at this point is going to be in board mounting and grounding, possibly to include power decoupling. You may find that one board radiates from the supply line, ground, or somesuch.


My take is that there will be a difference, but not anything you’ll reliably observe. That is; not too significant. Certainly not 10 dB worth. If you make the change and find a large difference, I’d look hard at the other changes you made.

Wait - do you have ground plane under the antenna?


No, she doesn’t afaict. Don’t look at the coloured layers on my drawing. They’re only to show how there’s minimal difference in distance from a surface pour to a prepreg pour. They represent different Z heights but nothing in XY.

No, of course not - I’ve followed Laird’s copper keepout instructions to the letter.

That was my thinking when I originally decided not to use pours, as my experience is that they’re more trouble than they’re worth, acting as unintentional radiators if poorly stitched and so forth.

My device is battery-powered and had no ohmic connections to the world during range testing afaik. Which raises the point that they really should be doing range testing with the dingus connected to its load - a big motor grounded to the metal enclosure). That’s likely to have a big impact, for better or worse. The Laird dev board was also battery-powered during range comparison testing AFAIK, with no connections. I need to double-check that they didn’t have it hooked up to a laptop, though, good point.

My vote is for ground plane impedance & distance to RF traces.

The dev board has a ground plane on the top layer, so with this arrangement it is a controlled distance between this and the (known during their RF design) distance to the RF traces on the module. This distance will affect transmission line impedances & matching etc. As you don’t have a GND plane on the top layer, the distance is the designed gap as above, plus whatever is added to the inner GND layer with your stackup.

Plus the ground path into the module with a top plane is just a huge area of copper == low inductance/resistance. With an internal plane (usually thinner) it is through a (relatively for RF) small number of vias which add impedance.

I know just enough about RF to believe these are important to look at, but not near enough to be confident in the % probability or level of impact! But they would still be my guess given everything else seems to match the dev board and the recommendations.