PCB antenna design problem: too short range?

RE: PCB antenna design problem: too short range?

Jørn — Fri, 11 Aug 2017 10:29:59 GMT

Hello Angel

As MANGO mentioned the traces leading to your balun are of different lengths, however I don't believe this will have a significant impact on the balun output.

My reasoning here is as follows. The pins of the nRF51 have a 0.4mm spacing. Using that as reference the difference in your trace lengths are 0.047mm for the emitter and 0.163mm for the receiver. With an approximate dielectric constant of 3.14 (assuming FR4 substrate, using 4.8 dielectric constant and finding the average substrate and air based on 1.6mm substrate height and approximately 0.16mm trace width) you get a phase difference of 0.25 degrees for the transmitter and 0.85 degrees for the receiver. This should have minimal impact on the output of the balun.

I believe the source of your loss is mismatch. You say you have copied the meander antenna of the dongle, but you have not copied the surrounding layout, nor used the pi network which is used in the design. For your design your chip will be matched to 50 Ohm through the balun, but your antenna is very likely not 50 Ohm. As both MANGO and Dave_couling mentioned in their comments this will have a huge impact on your signal attenuation.

An antenna is a very sensitive thing, whose impedance is dependent on its physical shape and proximity to other things in its environment (especially conductive materials). Having a good ground is paramount, preferably on the same layer as the antenna is located. Ground should ideally be in the form of a large unbroken ground plane, and should be connected with vias to the ground plane on the bottom layer, if present. The antenna should have a keep-out region around it, and there should be no traces or components present within this region.

The balun should have a unbroken ground plane underneath it on the bottom layer, as shown in the baluns datasheet (in the case of BAL-NRF02D3 as used in the nRF51 datasheet). If I interpret your layout correctly you have omitted this ground plane. This will likely affect the impedance of the balun, which also can cause mismatch and signal attenuation.

For a more thorough evaluation we would need to see your gerber/project files as well as schematics. If your design is confidential you can create a mypage case at www.nordicsemi.com and refer to this case in your ticket.

Best regards

Jørn Frøysa

RE: PCB antenna design problem: too short range?

Dave_couling — Thu, 10 Aug 2017 18:33:13 GMT

Adding a Pi-Network is critical to almost every RF design. The Balun only matches between the balun itself and the nRF chip, but like a transformer it needs an impedance matched load. Have you used a Network Analyzer to measure the matching of your Antenna?

More than likely, the unbalanced tracing to the balun, along with the un-tuned trace and antenna means you're getting high RF reflections on the board thats drastically affect your Transmitted RF.

RE: PCB antenna design problem: too short range?

MANGO — Thu, 10 Aug 2017 14:39:46 GMT

About there is a ground plane right below the antennas, Do you think that it is enough grounding?

Well, as far as I know, as mentioned in here, There shall be no ground plane on the PCB layer(s) beneath the antenna trace. No ground plane, PCB traces or components should be placed close to the antenna trace.

I think there was a confusion about Do you think that it is enough grounding?

The grounding was about top / bottom ground pour. However, that ground plane has to be kept out below the antenna.

So Jørn was asking that In other words, have you maintained a keep-out region on all layers underneath the antenna?

Can you upload the details about your PCB so that we can check the ground plane?

-Best Regards

RE: PCB antenna design problem: too short range?

MANGO — Thu, 10 Aug 2017 14:34:25 GMT

Hello, Angel. As mentioned, these (aligning the balun) are minor issues.

I was informed from the Nordic's distributor, so I don't know the exact math about this.

It will affect the antenna range, but it will be minor, compared to the effect due to the ground plane which is beneath the antenna.

I created a custom 4-layered PCB that used nRF52 and λ/4 printed monopole antenna.

This one had the above minor issue; I accidentally created a non-symmetric trace.

Using the DTM mode, the TX power from 2.4GHz (actually recorded 2.399987GHz) was -0.7dBm.

So you can speculate that this doesn't affect much.

RE: PCB antenna design problem: too short range?

Jørn — Thu, 10 Aug 2017 11:00:09 GMT

Hello Angel. Just to be clear, you say there is a groundplane underneath the antenna. Does the groundplane actually cover the area directly underneath the antenna itself? In other words, have you maintained a keep-out region on all layers underneath the antenna?

RE: PCB antenna design problem: too short range?

angel — Thu, 10 Aug 2017 10:01:31 GMT

Hi MANGO,

First of all, every answer is of very good help, thank you very much for your reply!

I see that you in the thread that you link, in the end, the decision of removing the Pi network is taken. We also have no laboratory equipment available to do these tuning measurements, so I assume that for us is also useless to put a pi network there.

As I wrote as a reply to my previous question, there is a ground plane right below the antennas, that is connected through these lanes that you see next to the antenna. Do you think that it is enough grounding?

About the centering of the Balun, do you think it will affect a lot if we align it? I mean, can it affect significantly to the range of the antenna?

Thanks again for your reply!

Best

RE: PCB antenna design problem: too short range?

angel — Thu, 10 Aug 2017 09:42:58 GMT

Hello Dave, thanks for your answer! We didn't use a Pi network because we thought that it was not necessary when we use the matching balun that we are using.

Also, we didn't use any impedance calculator, we just copied the design of the antenna from the development kit files (dongle nRF51), and tried to maintain our design as close as possible to that reference design.

About the grounding, just below the antenna we have a big ground plane, connected through vias to the lanes that you see in the picture above. Do you think this is sufficient as ground pour?

Thanks again Dave!

RE: PCB antenna design problem: too short range?

MANGO — Thu, 10 Aug 2017 07:30:19 GMT

Hi, Angel. I think there is a minor issue with the ANT1 (31) and ANT2 (32) pin.

it is important to state again that the PCBs are already in production, so a solution requiring minimum changes in hardware would be better.

Hmm, I hope for your understanding that my answer won't be a big help.

While waiting for a better solution / answer provided by the Nordic's dev-team, take a look at my answer, please.

This issue was detected from the Nordic's distributor when I was creating a custom PCB that uses nRF52832.

Take a look of the PCB traces of pin 31 and 32, please.

ref. Nordic devzone - PCB Antenna. Tuning not necesary

ref. Nordic Blog - General PCB design guidelines for nRF51

Both traces are symmetric; they are stretched with the same length and bent at the same y position.

As a result, the balun's center is aligned to the center of pin 31 and 32.

Also, as you see the blog's picture, there are plenty of ground vias at the nRF51 MCU footprint.

Whereas,

your trace is not symmetric. The trace of pin 31; it is bent "earlier".

So the balun's center is not aligned.

Also, I can't tell whether your PCB has sufficient ground vias at the nRF51 MCU footprint.

This type of issue has an effect on matching network.

Like "Dave" 's comment, have you used an impedance calculator?

Also, how is the ground pour configured below the matching network?

-Best Regards

RE: PCB antenna design problem: too short range?

Dave_couling — Wed, 09 Aug 2017 21:16:43 GMT

You need to add a Pi network after the Balun so you can tune the antenna. Did you use an impedance calculator to determine your trace width? Is this from a reference design? I hope you're design has a ground pour that was omitted from your photos. Reference ground size and consistency is crucial to good transmit efficiency.