Having both U.FL and Trace Antenna with Zero Ohm resistor?

[Jaimin Ajmeri]

We are thinking to evaluate both the U.FL and Trace Antenna options on a custom nRF52840 prototype board.

1. Referring to this discussion, point 3 is about provisioning two antenna types. I understand that by using zero ohm resistor i.e., by populating/de-populating the antenna type could be selected/unselected respectively.

2. However, in other discussion, leaving the resistor pads unconnected would impact the signal because the pads would act as transmission line.

Suggestion needed:

It's a 4 layer board, having calculated the trace-width for 50-ohm impedance matching trace using the parameters of the PCB fabricator. I have replicated the nRF52840-DK trace antenna and SWF connector connections.

1. I can think of this simple circuit with 0-ohm (R31 & R35) in series on both the antenna lines: (I need a suggestion for PCB layout for this circuit). With this approach, I guess the 0-ohm resistor would have a negative impact on RF signal because it would impact the 50-ohm impedance matching trace.

2. The other option, is to have two LC networks as seen above with 0-ohm connected to nRF_ANT pin.

This is Work In Progress, replicating nRF52840 DK antenna and SWF connector traces:

[Jaimin Ajmeri]

I was looking for modules with both the antenna types, I stumbled upon this on LCSC site the part is E73-2G4M040S1D. On page 11 of its user manual, I found the image of populating one resistor to choose the antenna type.

I guess it's a 0-ohm resistor. The orientation of that resistor selects the antenna.

From the above image, I think this should work because there are 3 pads out of which the common pad is connected to nRF52840's Antenna pin, and the other two pads go to respective antenna types.

Can someone confirm if this is a good idea for prototyping?

[Marjeris Romero]

Hi Jaimin,

Very sorry for the lack of reply on this post. I found it in my queue today. Using a 0R resistor to choose between antennas is a very common design choice amount our customers, nothing wrong with that, but you need to be aware on how you are placing the 0R resistor so you don't create an open stub as it's mention in https://devzone.nordicsemi.com/f/nordic-q-a/27478/is-50-ohm-maintained-at-ufl-connector/108532#108532

In the discussion above my recommendation to the customer would be to move R7 to the right so you can solder one pad of the resistor directly on the RF path coming from the ANT pin, this way you will not have the stub coming out of the RF path when the resistor is desoldered:

And also add a series resistor on the RF path as well as it's describe on the same answer on the case above: "Use two components in a T-junction configuration to choose between either antenna or conductor. You should then try to keep it as small as possible, and keep in mind that parasitics from the resistor could affect your match."

In the case of the module on your picture I am supposing the feeding line from the ANT pin is coming from under the module:

This looks like an OK solution but having a 90 degrees on the RF path can also potentially create other challenges because of reflections on the RF path.
The best solution as discussed in case ID 27478  would be using a connector with a built in switch placed as part of the transmission line leading out to the antenna as used in the nRF52840 DK, but if not possible I think both option 1 (as long as the resistors are placed close to each other so the stubs are minimized) and option 2 (with 90 degrees RF paths) are OK solutions.

About your other question:

1. I can think of this simple circuit with 0-ohm (R31 & R35) in series on both the antenna lines: (I need a suggestion for PCB layout for this circuit). With this approach, I guess the 0-ohm resistor would have a negative impact on RF signal because it would impact the 50-ohm impedance matching trace.

You cannot have 2 radio matching networks (as seen in option 2), as you need to placed the radio matching components very close to the ANT pin and follow the spacing and dimentions shown in the reference design as close as possible, so you need to go for alternative 1:

nRF_ANT pin > Radio matching components > T-junction of 0R to choose between antenna and uFL connector (if not using a switching connector) > antenna


Best regards,

Marjeris

 

[Jaimin Ajmeri]

Marjeris Romero said:

nRF_ANT pin > Radio matching components > T-junction of 0R to choose between antenna and uFL connector (if not using a switching connector) > antenna

Thanks for answering Marjeris Romero

Your answer is clear to me. I would go with option 1.

Thanks for informing me about the 90 degrees RF Path reflections. I would follow the T-Junction, meaning placing u.FL connector on the left side from the antenna pin as per your image. This answers my question.

Few More Questions:

I would like to know more about the trace antenna PCB layout. I use KiCAD for my project. The footprint library has a few PCB trace antennas as footprints.

1. In KiCAD the TI SWRA117D type footprint is readily available. Would you suggest using it?

https://github.com/KiCad/kicad-footprints/tree/master/RF_Antenna.pretty
https://www.ti.com/lit/an/swra117d/swra117d.pdf

2. I came across the reference design layout GitHub repository. The "Library/Nordi_Misc.lbr" has the trace antenna layout as on the nRF52840-DK, would you recommend using it? Note: I have used SnapEDA to convert from Eagle format to KiCAD format.

https://github.com/NordicPlayground/nrf5-eagle-reference-design/tree/master/Library

3. If 2 is recommended, I see that the library has multiple footprints distinguished by length (-1, -2, +0, +1, +2, +3, +4). Which is the one used by the nRF52840-DK? Which do I choose?

[Jaimin Ajmeri]

Marjeris Romero please look into my other questions if you can.

Jaimin Ajmeri said:

Few More Questions:

I would like to know more about the trace antenna PCB layout. I use KiCAD for my project. The footprint library has a few PCB trace antennas as footprints.

1. In KiCAD the TI SWRA117D type footprint is readily available. Would you suggest using it?

https://github.com/KiCad/kicad-footprints/tree/master/RF_Antenna.pretty
https://www.ti.com/lit/an/swra117d/swra117d.pdf

2. I came across the reference design layout GitHub repository. The "Library/Nordi_Misc.lbr" has the trace antenna layout as on the nRF52840-DK, would you recommend using it? Note: I have used SnapEDA to convert from Eagle format to KiCAD format.

https://github.com/NordicPlayground/nrf5-eagle-reference-design/tree/master/Library

3. If 2 is recommended, I see that the library has multiple footprints distinguished by length (-1, -2, +0, +1, +2, +3, +4). Which is the one used by the nRF52840-DK? Which do I choose?

[Marjeris Romero]

Hi,

I am sorry for not getting back to you. Which PCB antenna design you choose is totally up to you, both designs are good alternatives depending on what you are looking for. You can use any known PCB antenna designed for 2.4GHz and achieve good range and performance.

It's important that you follow the antenna design closely though, and it's also recommended to use the same thickness and type of PCB material used in any reference design of the antenna design your are using.

You will anyways need to tune the choosen antenna to your own board. I recommend you add some extra length so the antenna can be made slightly shorter when tuning.

As a general rule, a longer (full sized) antenna will give you better performance than a cut down or shrinked antenna, so if you have space in your design I would recommended to use a 1/4 wave monopole antenna (as the one used in the nRF52840 DK). You can find a whitepaper about how to design your own quarter wave antenna here.

You should also consider the size of the ground plane in your board. A small ground plane will lead to less antenna gain, no matter what antenna you use. A meander antenna (as the one used in the TI dongle) takes less space so it's a popular choice for USB dongles and other small PCBs, but a dongle will benefit from the added ground plane in a the PC so you can have OK performance with a small antenna. Using this antenna in a small PCB will give you less range than using a 1/4 wave antenna.

I don't know if you shared the size of the PCB you are making, but based on all this I will go for the f-inverted meander if you have a small PCB or module which will be connected to a larger ground plane, or if your PCB is larger and you have the space go for a 1/4 wave monopole antenna.

Best regards,

Marjeris