PCB antenna design problem: too short range?

[angel]

Dear Nordic,

Some time ago we started a project in which we decided to use ANT protocol to communicate wirelessly. However, now that we are going to production in a very very short time, we have spotted a very critical problem in the range of the communication.

Here is the design of the antennas, in emitter and receiver pcb designs:

And here is the schematic for both of them:

The total length of the antenna is 28.13 mm and the width 0.35 mm.

The main problem is that we only have like 1 to 1.5 meters of acceptable range. If I use the nordic DK as TX end, the range is significantly bigger, like 4 to 5 meters. This would be enough for our application.

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

We have already tried different frequency numbers by SW (from 2400 MHz to 2524 MHz), but that only helped a bit (2433 MHz) seems to work a bit better.

Also changed the RADIO_TX_POWER to +4dBm but didn't really do anything.

Anyone has any idea how we could improve the range of our antenna? Again, I know that the same software using the DKs has a really good performance.

Thank you very much for your help.

[MANGO]

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.

[MANGO]

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

[Dave_couling]

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.

[Jørn]

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