2.4GHz antenna design

[_Sinusoidal]

Hello, I'm designing a PCB that has a NRF24L01+ transceiver (2.4GHz) controlled with an Atmega328P. I've been doing reading about how to properly design the PCB layout in the RF transceiver area, but I haven't been able to find any information regarding trace path angles and if they have any effect on the performance of the antenna. I have attached a snapshot of the basic layout of my components and how I would like to route my traces. Are the bends in the antenna trace going to cause any sort of interference in the signal path?



Any advice is greatly appreciated! Thanks!

[krapht]

It's hard to tell with these things, and should really be checked in simulation. The problem with 90 degree bends is excess capacitance which causes the track impedance to change. On the other hand, you're using a chip antenna, which tells me max transmit range isn't the biggest deal. So just go for it and revisit the issue if you don't get the performance you need.

FWIW whenever I do an RF layout I always use curved traces of at least 5x track width in radius. Mostly because I hate cluttering my schematics with useless RF layout symbols like "90 deg miter", and the fact that trying to etch a precise miter in a track that's made to +-20% tolerance is an exercise in futility. And I'm kind of OCD about having the schematic be the master diagram for the PCB, so there's no helping it, haha.

[Howardlong]

Is there not a reference design? I'd seriously take that together with the board layer stack up and save yourself the fear of the uncertainty of the unknowns.

[uncle_bob]

Hi

What board material are you planning to use? FR4 is pretty wierd stuff at 2.4 GHz. The "good stuff" costs a bit more ...Until you have that sorted out, working out trace issues is not worth messing with.

Bob

[_Sinusoidal]

Thanks for the feedback guys. I moved around a couple of the parts to shorten the trace length. As suggested my next step should be to run a simulation I suppose?

It's hard to tell with these things, and should really be checked in simulation. The problem with 90 degree bends is excess capacitance which causes the track impedance to change. On the other hand, you're using a chip antenna, which tells me max transmit range isn't the biggest deal.

Is there any free software available out there that can do these sorts of simulations? Any you recommend?

You're right, max transmit range is not one of my goals for this project. In reality the transceivers that are communicating will be maybe 2 meters apart. I just want to make sure that the design is robust and doesn't bite me in the ass later.

Is there not a reference design? I'd seriously take that together with the board layer stack up and save yourself the fear of the uncertainty of the unknowns.

I have looked at references from the manufacturer and also breakout board products for this device. My main issue is size constraint. The way these components are oriented are one of the few configurations possible, given my size specifications and other components on the board.

What board material are you planning to use? FR4 is pretty wierd stuff at 2.4 GHz. The "good stuff" costs a bit more ...Until you have that sorted out, working out trace issues is not worth messing with.

I actually did not know that the board material is a significant factor. This is my first PCB design that includes signal frequencies >1GHz. I was intending to just use FR4, can I get away with that considering I'm not going for super high performance? My transmit range will be less than 10 meters, and probably only use 250Kbps to 1Mbps data rates.

[_Sinusoidal]

Forget about simulation, if you do not have $$$$. Tools for that kind of physical simulation (hyperlynx, ansys maxwell q3d, ads, awr, comsol or equivalent) are not cheap.

Do whatever you can to conform to existing designs you can find on the internet, or refer to Nordic's ref design. There is virtually no way to verify your design before building it.

This is a low budget project, so yeah, purchasing software is likely not possible. I'm trying my best to follow all guidelines I can find online, and to stay close to Nordics recommendations. My largest concern is whether or not these 90 degree bends will cause significant performance problems, as they are basically mandatory in my design.

[uncle_bob]

Hi

What board material are you planning to use? FR4 is pretty wierd weird stuff at 2.4 GHz. The "good stuff" costs a bit more ...Until you have that sorted out, working out trace issues is not worth messing with.

Bob

All consumer 2.4G devices are build on FR4, and they do their jobs (tline, antenna, directional coupler, combiner) well.

Hi

But.... they spend significant time characterizing the material they are going to use.  It's not something you can read off a data sheet, and it's not consistent manufacturer to manufacturer.

Bob

[Howardlong]

Is there not a reference design? I'd seriously take that together with the board layer stack up and save yourself the fear of the uncertainty of the unknowns.

I have looked at references from the manufacturer and also breakout board products for this device. My main issue is size constraint. The way these components are oriented are one of the few configurations possible, given my size specifications and other components on the board.

My bold... I strongly suspect that the layout is done for a reason. I notice from your layout that there is little in the way of ground plane for example and parts are located directly adjacent to stitching. There is also no apparent adherance to any controlled impedance traces.

You may well find it works "well enough", but equally I wouldn't be surprised if it worked just as well without any of those lumped parts at all which are there for a balun filter to match an unbalanced load impedance to a balanced source impedance.

If you are serious about size, how about using a pre-baked balun filter like this one which offers 50 ohm unbalanced directly to,your antenna? http://www.johansontechnology.com/datasheets/baluns/Johanson%20nRF24L01_nRF24L01+_App_Note.pdf

Judging from the roigh sizing of the CPW feed, it looks to be less than 1.6mm if it's double sided, more like a 0.8mm substrate.

[_Sinusoidal]

I notice from your layout that there is little in the way of ground plane for example and parts are located directly adjacent to stitching. There is also no apparent adherance to any controlled impedance traces.

I had not really got to focusing on the grounds at that point, was more wondering about the effects of the right angles in the signal path. I have heard that they can cause reflections which results in destructive interference. I think I need to do some reading on waveguides.

Is there a rule of thumb for how far components should be from ground plane stitches?

If you are serious about size, how about using a pre-baked balun filter like this one which offers 50 ohm unbalanced directly to,your antenna? http://www.johansontechnology.com/datasheets/baluns/Johanson%20nRF24L01_nRF24L01+_App_Note.pdf

I have never heard of these before, very cool! I may actually add this to my design instead, these chips are being sold at a pretty good price. Not sure why I haven't seen these recommended before? Do you know of any potential risks of using these, besides a slightly higher cost? Having 5 less components would be nice...

Judging from the roigh sizing of the CPW feed, it looks to be less than 1.6mm if it's double sided, more like a 0.8mm substrate.

I'm sorry, I don't think I have enough background knowledge to understand what you mean by this. Are you talking about the trace width of the output to the antenna? Is this supposed to be a specific size depending on the substrate thickness and dielectric constant? I haven't really studied this stuff too comprehensively in school yet.

The board is just double sided and I originally intended it to be 1.6mm thick.



Thanks for the info, on a huge learning curve right now so I appreciate the help a lot.

[Howardlong]

I notice from your layout that there is little in the way of ground plane for example and parts are located directly adjacent to stitching. There is also no apparent adherance to any controlled impedance traces.

I had not really got to focusing on the grounds at that point, was more wondering about the effects of the right angles in the signal path. I have heard that they can cause reflections which results in destructive interference. I think I need to do some reading on waveguides.

Is there a rule of thumb for how far components should be from ground plane stitches?

The ground plane fill on all planes is a fundamental part of the design, and needs to be considered from the ground up (oops, pun), not as an afterthought I'm afraid: you need to look at it as a system. Those parts are spaced out like they are for many reasons including cross coupling and parasitics.

If you are serious about size, how about using a pre-baked balun filter like this one which offers 50 ohm unbalanced directly to,your antenna? http://www.johansontechnology.com/datasheets/baluns/Johanson%20nRF24L01_nRF24L01+_App_Note.pdf

I have never heard of these before, very cool! I may actually add this to my design instead, these chips are being sold at a pretty good price. Not sure why I haven't seen these recommended before? Do you know of any potential risks of using these, besides a slightly higher cost? Having 5 less components would be nice...

Judging from the roigh sizing of the CPW feed, it looks to be less than 1.6mm if it's double sided, more like a 0.8mm substrate.

I'm sorry, I don't think I have enough background knowledge to understand what you mean by this. Are you talking about the trace width of the output to the antenna? Is this supposed to be a specific size depending on the substrate thickness and dielectric constant? I haven't really studied this stuff too comprehensively in school yet.

The board is just double sided and I originally intended it to be 1.6mm thick.



Thanks for the info, on a huge learning curve right now so I appreciate the help a lot.

There is a reason to use thinner substrate as the controlled impedance feeds are narrower with thinner board (narrrower traces == smaller board). The alternative is to go multilayer and use an embedded ground plane.

There's a very rough rule of thumb for FR4 (approx Er=4.0) that for a 50 ohm microstrip trace, the thickness is double the board thickness, so for 1.6mm that's a 3.2mm trace. That's a big trace! Look for microstrip calculators online. An alternative to microstrip is coplanar waveguide which is more demanding in that it demands plenty of via stitching but is generally considered less lossy and provides better isolation. For the distances you're talking about I'd stick with microstrip, but keep your parts and traces away from adjacent ground flooding on the same plane or you'll end up with a hybrid CPW/microstrip.

For 0.8mm FR4, you can halve the trace width to a more manageable 1.6mm trace, but for home-made boards I regularly have to go to 0.4mm board thickness for the sort of packages like the nrf24l01 to be able to logistically fan out the package reasonably. The physical rigidity of these thinner boards is of concern for production: you're better off with four or more layers, where the effective dielectric thickness might typically be only be 0.25mm (board stackup varies widely, so always check with your board house!) making it a far more sensible option as 0.5mm traces are easy to route, and as luck would have it are very close to 0402 pad sizes for your matching components. Also note that typical reference designs for PCB antennas are frequently on a 1.6mm substrate.

When transitioning from a small land to a controlled impedance microstrip, start it as close to the land as logistically possible so that the uncontrolled impedance is minimised, and do it gently, with say, a 45 degree "funnel" rather than an abrupt width change.

The nice thing about that integrated balun filter other than its small physical size is that you now have a standard 50 ohm interface to route to any one of a gazillion different antenna layout designs.

[krapht]

Since you've spoken more about your background with RF PCB layout, I highly highly recommend you copy the PCB layout from any manufacturer's relevant application note at your target frequency! Even if this particular chip doesn't have one, I know there are many chip antenna layouts out there for various RF transceivers. It's simply a matter of, you do not have the resources to troubleshoot your design if it should happen to not work.

Ceramic chip antennas are notorious for being easily detuned, set yourself up for success by minimizing the things you need to check when you have this produced.

[Koen]

Don't overthink it. The differential pair is well routed and that's the only thing required here. Your antenna placement, ground area, copper weight, dielectric material, components and so on will be different from the antenna manufacturer and chip manufacturer datasheets anyway.

The only meaningful thing you can do is to later borrow a VNA to match the antenna and verify the balun.

JTI single package baluns are great.

[_Sinusoidal]

For 0.8mm FR4, you can halve the trace width to a more manageable 1.6mm trace, but for home-made boards I regularly have to go to 0.4mm board thickness for the sort of packages like the nrf24l01 to be able to logistically fan out the package reasonably. The physical rigidity of these thinner boards is of concern for production: you're better off with four or more layers, where the effective dielectric thickness might typically be only be 0.25mm (board stackup varies widely, so always check with your board house!) making it a far more sensible option as 0.5mm traces are easy to route, and as luck would have it are very close to 0402 pad sizes for your matching components. Also note that typical reference designs for PCB antennas are frequently on a 1.6mm substrate.

Thanks again for the great info! You've convinced me to go with the integrated balun filter, it just makes sense in terms of its size and ease of use. So now, as I understand, I still require a controlled impedance trace between the balun and the chip antenna. Sparkfun, from what I can see, has a 2 layer breakout board (looks thick, maybe 1.6mm?) that has their chip antenna connected almost directly to their balun setup.



The trace between their balun and chip does not look to be very wide at all... is this because of how short the trace is? Would I be able to do something similar?



I have changed my design to more closely resemble the app notes in the balun datasheet HowardLong linked me to, as well as Sparkfuns breakout board. I have not yet added in all the ground vias, and there are still some other missing connections. I'm hoping someone could provide me with their opinion on whether or not I will be able to get away with a very short uncontrolled impedance trace between the balun and antenna.

Since you've spoken more about your background with RF PCB layout, I highly highly recommend you copy the PCB layout from any manufacturer's relevant application note at your target frequency! Even if this particular chip doesn't have one, I know there are many chip antenna layouts out there for various RF transceivers. It's simply a matter of, you do not have the resources to troubleshoot your design if it should happen to not work.

Ceramic chip antennas are notorious for being easily detuned, set yourself up for success by minimizing the things you need to check when you have this produced.

I mentioned earlier that I have size constraints that restrict me from simply copying other designs exactly. I'm trying to get my design as close to those references as possible, while still complying to my own size specifications. I'm also not going for super high performance, as my max transmit range will be less than 10 meters. This is why I have selected the chip antenna, as it provides a good mid ground between solution area and performance.

[Koen]

Yes, the shorter the track, the less impedance is a concern. Yet, if you have the surface for it, increase the track width closer to a 50ohm track.

[Koen]

If you can later borrow a VNA to verify your work, add a series footprint and a parallel footprint between the balun and antenna. It will allow you to add capacitors and/or inductors to match the antenna to 2.4GHz.

The antenna will behave differently depending on a lot of things and its center frequency will "move". In this datasheet of a similar 2.450 antenna by JTI, notice how the return loss at 2.450 is -2 without matching but -18 with.

Also, if you have ground planes on both sides of the board, sprinkle vias all over to tie them together.

[_Sinusoidal]

If you can later borrow a VNA to verify your work, add a series footprint and a parallel footprint between the balun and antenna. It will allow you to add capacitors and/or inductors to match the antenna to 2.4GHz.

The antenna will behave differently depending on a lot of things and its center frequency will "move". In this datasheet of a similar 2.450 antenna by JTI, notice how the return loss at 2.450 is -2 without matching but -18 with.

Also, if you have ground planes on both sides of the board, sprinkle vias all over to tie them together.

I likely will not be able to get my hands on a VNA any time soon.  Trying to get my design as theoretically sound as possible, as I won't be able to verify it's performance other than whether it is working or not. Thank you for the pointers, I will make that uncontrolled trace as fat as possible and cross my fingers... unless someone comes along with a strong objection to that.

[Howardlong]

In that case I'd just go for it. I don't know why you have physical space constraints, but my most successful product is space constrained as part of the original design criteria, and that form factor has given the product a USP as a result for several years.

[_Sinusoidal]

In that case I'd just go for it. I don't know why you have physical space constraints, but my most successful product is space constrained as part of the original design criteria, and that form factor has given the product a USP as a result for several years.

I'm more or less trying to get the board size down to a practical minimum, the design criteria calls for it. I always have appreciated products with tiny form factors, they often have elegant design ideas. Glad to hear yours has been a success. Thanks again for the help, it is much appreciated.