Author Topic: 2.4GHz PCB antenna design verification  (Read 1577 times)

0 Members and 1 Guest are viewing this topic.

Offline ASHU

  • Contributor
  • Posts: 32
2.4GHz PCB antenna design verification
« on: August 08, 2017, 05:00:02 PM »
Hello everyone,

I have designed a PCB with a 2.4GHz PCB antenna on it. I have no experience with antenna designing ( but have recently gained a little bit knowledge after reading a lot online).
With all the things I could understand regarding antenna designing, I made a PCB design and would like to know from the experts here if the design is ok or not. I am attaching the board file images as well as few other files for your understanding as to what I am trying to achieve. Impedance is 50ohm.


There are few things I am unsure about
1. I read a few places that the bottom layer of PCB should not have any components on it (for antenna performance purpose) and you should try to work on a four layer board. Where in that is not the case with me. Unfortunately four layer boards increase the cost of production and are also tough to design . How will my antenna perform in this condition, any rough guess after viewing the images?

2. The top and bottom layer both have ground planes, but along with all the components (according to the PCB bottom & PCB top) is the design alright or do I need to move the antenna upwards to cover more ground path just below it. I am trying to make the PCB as small as possible. Although I have tried to eliminate any signal just below the antenna trace path.

3. In PCB top.png, (Antenna trace from IC  to capacitor)  before the trace join with the capacitor's SMD pad, the area below the trace is not filled with ground. Will it do or do I need to cover up that also?

To achieve the 50ohm impedance  I have used coplaner wavelength calculator to calculate the trace width (0.797 mm) and distance between RF trace and ground (0.15mm) .
The PCB height is 0.8mm (0.710 dielectric height & Er of 4.3 - received from my manufacturer) Refer image (cal1 & cal2)

Is the design good to go or not?

Thank you
 

Offline janekm

  • Supporter
  • ****
  • Posts: 419
  • Country: gb
Re: 2.4GHz PCB antenna design verification
« Reply #1 on: August 08, 2017, 05:38:57 PM »
2-layer is fine for such a short transmission line. But, you have a broken ground plane beneath the transmission line, which is not good (and you should be able to avoid that).

In my experience it will still work (maybe -10dB less performance) but it could be better. Also try to make sure your ground plane is as solid (un-interruped) as possible. The antenna design you are using is dependent on the ground plane next to it.
 
The following users thanked this post: ASHU

Online T3sl4co1l

  • Super Contributor
  • ***
  • Posts: 9321
  • Country: us
  • Expert, Analog Electronics, PCB Layout, EMC
    • Seven Transistor Labs
Re: 2.4GHz PCB antenna design verification
« Reply #2 on: August 08, 2017, 06:25:49 PM »
Sorry, but you need to get your priorities in order:


I have designed a PCB with a 2.4GHz PCB antenna on it. I have no experience with antenna designing ( but have recently gained a little bit knowledge after reading a lot online).

1. You have no experience with design.  This isn't a problem in the long run, but it's a cost.  It could take weeks to years to become familiar with antenna and transmission line theory (depending on how familiar one needs to be).  In the course of that, you'd learn the tools necessary to execute a design confidently: EM field solvers, microwave simulators, how to use a VNA and evaluate the finished device, etc.

Besides the project timeline cost, you'd incur at least as much labor in the process, or school expenses (for a more classical education).  It's not a cheap process, however you slice it!

(To say nothing of regulatory testing.)

Which brings up your second concern:

Quote
1. I read a few places that the bottom layer of PCB should not have any components on it (for antenna performance purpose) and you should try to work on a four layer board. Where in that is not the case with me. Unfortunately four layer boards increase the cost of production and are also tough to design . How will my antenna perform in this condition, any rough guess after viewing the images?

2. If you are doing a few-off build, the cost of a 32-layer board is still far exceeded by the cost of designing and evaluating this properly!

If this is going into small production (~1000s/yr?), the cost of development is still greater than the PCB cost, no matter what you use.

If this is going into higher production (>10k/yr?), the FCC will hear about it sooner or later, and regulatory approval will be critical.  Tack on another $10 or 20k of lab time.

(Note that, you technically need regulatory approval if you're selling more than one, period.  Most companies do regulatory approval for their standard products.  You might get away with selling thousands over many years, without approval.  And I've seen this happen before.  As with all things, it's a business decision: do you want to get stuck with C&D letters, frozen sales, or fines, at some point?  Is that risk worthwhile?)

3. Use a pre-cooked module.

These are CHEAP.  Like ten bucks cheap.  Even less from China.  Even the Chinese ones are FCC and CE approved.  As long as you follow the usage for the module, you don't need to test your finished product as an intentional radiator.

You don't incur any project timeline impact (or, at most, a few days to shop for one, make the footprint, and pick up the basics on programming it).  The BOM cost is marginal.  You can use 2-layer boards without worry (no RF touches the board, aside from the antenna being along the edge; or, at worst, a pin is provided which goes to a coax connector for an approved antenna type, and all you need is a short trace, connector, and lots of vias and ground pour).

As you can see, there are many good reasons why modules are so popular!

Tim
« Last Edit: August 08, 2017, 06:27:36 PM by T3sl4co1l »
Seven Transistor Labs, LLC
Electronic Design, from Concept to Layout.
Need engineering assistance? Drop me a message!
 
The following users thanked this post: ASHU

Online MarkF

  • Frequent Contributor
  • **
  • Posts: 601
  • Country: us
Re: 2.4GHz PCB antenna design verification
« Reply #3 on: August 08, 2017, 06:28:17 PM »
You may want to check out the antenna on the nRF24L01 2.4GHz Transceiver.
 

Offline ASHU

  • Contributor
  • Posts: 32
Re: 2.4GHz PCB antenna design verification
« Reply #4 on: August 08, 2017, 08:41:16 PM »
Thanks everyone for the valuable input.

2-layer is fine for such a short transmission line. But, you have a broken ground plane beneath the transmission line, which is not good (and you should be able to avoid that).

In my experience it will still work (maybe -10dB less performance) but it could be better. Also try to make sure your ground plane is as solid (un-interruped) as possible. The antenna design you are using is dependent on the ground plane next to it.

What looks like broken ground on the top layer is connected from bottom layer. So, I suppose that will do...right ?.
If you think it can be better. Can you please point out few places where I could improve the design?



1. You have no experience with design.  This isn't a problem in the long run, but it's a cost.  It could take weeks to years to become familiar with antenna and transmission line theory (depending on how familiar one needs to be).  In the course of that, you'd learn the tools necessary to execute a design confidently: EM field solvers, microwave simulators, how to use a VNA and evaluate the finished device, etc.

Besides the project timeline cost, you'd incur at least as much labor in the process, or school expenses (for a more classical education).  It's not a cheap process, however you slice it!


I am trying to learn about all the terminologies. I know I am not an expert in this but I think the sooner I'll start the better. But what's the labour cost in this? Yeah PCB fabrication is there but what else?


(Note that, you technically need regulatory approval if you're selling more than one, period.  Most companies do regulatory approval for their standard products.  You might get away with selling thousands over many years, without approval.  And I've seen this happen before.  As with all things, it's a business decision: do you want to get stuck with C&D letters, frozen sales, or fines, at some point?  Is that risk worthwhile?)

3. Use a pre-cooked module.

These are CHEAP.  Like ten bucks cheap.  Even less from China.  Even the Chinese ones are FCC and CE approved.  As long as you follow the usage for the module, you don't need to test your finished product as an intentional radiator.

You don't incur any project timeline impact (or, at most, a few days to shop for one, make the footprint, and pick up the basics on programming it).  The BOM cost is marginal.  You can use 2-layer boards without worry (no RF touches the board, aside from the antenna being along the edge; or, at worst, a pin is provided which goes to a coax connector for an approved antenna type, and all you need is a short trace, connector, and lots of vias and ground pour).

As you can see, there are many good reasons why modules are so popular!

Tim

I am trying to reduce the size of my design. As you can see my attachments also (There are a few places where the pads of the QFN package are missing. Since they were not required and I removed them so that I can pass few wires from that area). Therefore I trying to avoid modules, and as you said that learning this thing can take weeks to years that's why I am here, so that I can reduce my project's timeline and on the other hand read a few books also in my spare time to get better at this.

And regarding FCC, as of not I am not thinking about going for higher production. And in case if the production increases (which we would really want), it will also mean that our sales are high, therefore more money....which will get us through certifications since we can hire expects and buy high end instruments also(I only have an oscilloscope now). There can always be version 2  :P

You may want to check out the antenna on the nRF24L01 2.4GHz Transceiver.

Yes I have, but is there a significant performance difference between the antenna you mentioned and the new nodemcu antenna? (attaching image below) I am using this because of it's low height and found it on sparkfun's rf library for eagle on github

 

Offline LaserSteve

  • Frequent Contributor
  • **
  • Posts: 583
  • Country: us
Re: 2.4GHz PCB antenna design verification
« Reply #5 on: August 09, 2017, 12:16:36 AM »
Or just hire  Kent, WA5VJB who does it for a living, and has the test gear and antenna range  to verify and improve your design before manufacturing.

www.wa5vjb.com

Otherwise buy the completed module, as the radiation pattern will probably drastically change when you install your design in a target unit.

I have a 2-18 Ghz sweeper, multiple return loss bridges, harmonic generators, RF detectors, test horn antennas, a very expensive bolometer power meter, a spectrum analyzer with a down-converter, just for my microwave ham radio hobby, and I'm still  less then then a third of the way to what I'd need to do FCC certification...
 
Steve


 

Offline Gribo

  • Regular Contributor
  • *
  • Posts: 208
  • Country: ca
Re: 2.4GHz PCB antenna design verification
« Reply #6 on: August 09, 2017, 12:16:58 AM »
Looking at your layout, I got few questions:
1. Why did you use an 0805 capacitor on the RF feed? Parasitic capacitance might be too high for a 2.4GHz feed.
2. Why did you place the crystal so far from the IC's inputs?
3. How do you plan to tune the design for your specific enclosure?
 

Offline ASHU

  • Contributor
  • Posts: 32
Re: 2.4GHz PCB antenna design verification
« Reply #7 on: August 09, 2017, 01:05:27 AM »

Looking at your layout, I got few questions:
1. Why did you use an 0805 capacitor on the RF feed? Parasitic capacitance might be too high for a 2.4GHz feed.
2. Why did you place the crystal so far from the IC's inputs?
3. How do you plan to tune the design for your specific enclosure?


1. It is as per the design guidelines. I am using an esp8266 , and the resistor is 0603
2. Waaooo...Is that also far away? Crystal is the one on the right hand side of the QFN package (U2 ->SMD pads) Just on the edge.
3. I was thinking about something like this https://espressif.com/sites/default/files/documentation/esp8266-hardware_matching_guide_en.pdf
I am thinking of adding the LC circuit only on 5-6 PCB's for testing purpose inside the enclosure, and making the changes (if required) in the final design

@ LaserSteve
For startup's, Certification is not a very big deal in my country. Eventually you will have to get it done but there will be some relaxed norms for startups
 

Offline janekm

  • Supporter
  • ****
  • Posts: 419
  • Country: gb
Re: 2.4GHz PCB antenna design verification
« Reply #8 on: August 10, 2017, 04:49:52 PM »
Thanks everyone for the valuable input.

2-layer is fine for such a short transmission line. But, you have a broken ground plane beneath the transmission line, which is not good (and you should be able to avoid that).

In my experience it will still work (maybe -10dB less performance) but it could be better. Also try to make sure your ground plane is as solid (un-interruped) as possible. The antenna design you are using is dependent on the ground plane next to it.

What looks like broken ground on the top layer is connected from bottom layer. So, I suppose that will do...right ?.
If you think it can be better. Can you please point out few places where I could improve the design?

(snip)

Sorry, I didn't explain that very clearly. You are using what's called a "microstrip" transmission line between your radio chip and the antenna layout. This one depends on having a solid ground plane beneath it, otherwise the impedance will change, causing a reflection of the signal. You really want to try and keep the groundplane underneath the microstrip as solid as possible.

In general it's good practice for a 2-layer microwave PCB to keep the "bottom" layer as solid ground as is possible, for several reasons. If you need to have a trace cross the bottom ground layer, try and keep it short, and avoid having big "slots" in that ground plane (these can act as unintentional slot antennas). Another reason is that you don't want currents in the ground plane have to travel around the slot, leading to high frequency voltage offsets (again leading to EMC issues).

Some of the comments here about needing to get a university-level education in microwave circuit theory and antenna design to get a simple 2.4GHz transceiver working are a little over to top for my taste (smacks of elitism).
I don't have a formal background in any of that, but I have passed multiple products based on 2.4GHz transceivers that I designed following basic rules of thumb and public antenna designs through EMC and intentional emitter (CE & FCC) testing, always with a good margin. Both with UK and Chinese test labs. It's not actually that hard to pass the tests if you follow the transceiver vendor recommendations and good practice.

On the other hand some of the radio modules from China (like the little one with the 2x4 pin header posted in this thread) are terribly designed and will likely make your product fail testing (a module like that is pretty terrible from an EMC point of view)! I certainly wouldn't use them as an example of good practice.
 

Online Ice-Tea

  • Frequent Contributor
  • **
  • Posts: 747
  • Country: be
    • Freelance Hardware Engineer
Re: 2.4GHz PCB antenna design verification
« Reply #9 on: August 10, 2017, 06:02:43 PM »
Not going to partake in the entire discussion, just putting out there that you can use ceramic antennae as well. These take away at least some uncertainty from your design and are probably even more compact. Example:

http://www.vishay.com/chip-antenna/list/product-45218/
An engineer never has a problem. He just needs more time.

FS: LeCroy SDA100G (50GHz and 20GHz + TDR module availble), Chroma 6304 + 2 x 63006, TTi TSX1820P, Yokogawa DL9240L (4ch 1.5GHz), TDS754D, Infinium 54815A, 54825A,R&S CMU 200, HP 8560E with tracking gen
 

Offline ASHU

  • Contributor
  • Posts: 32
Re: 2.4GHz PCB antenna design verification
« Reply #10 on: August 10, 2017, 06:12:14 PM »

Sorry, I didn't explain that very clearly. You are using what's called a "microstrip" transmission line between your radio chip and the antenna layout. This one depends on having a solid ground plane beneath it, otherwise the impedance will change, causing a reflection of the signal. You really want to try and keep the groundplane underneath the microstrip as solid as possible.

In general it's good practice for a 2-layer microwave PCB to keep the "bottom" layer as solid ground as is possible, for several reasons. If you need to have a trace cross the bottom ground layer, try and keep it short, and avoid having big "slots" in that ground plane (these can act as unintentional slot antennas). Another reason is that you don't want currents in the ground plane have to travel around the slot, leading to high frequency voltage offsets (again leading to EMC issues).

Some of the comments here about needing to get a university-level education in microwave circuit theory and antenna design to get a simple 2.4GHz transceiver working are a little over to top for my taste (smacks of elitism).
I don't have a formal background in any of that, but I have passed multiple products based on 2.4GHz transceivers that I designed following basic rules of thumb and public antenna designs through EMC and intentional emitter (CE & FCC) testing, always with a good margin. Both with UK and Chinese test labs. It's not actually that hard to pass the tests if you follow the transceiver vendor recommendations and good practice.

On the other hand some of the radio modules from China (like the little one with the 2x4 pin header posted in this thread) are terribly designed and will likely make your product fail testing (a module like that is pretty terrible from an EMC point of view)! I certainly wouldn't use them as an example of good practice.

Okay, Thank for the help. I was quite eager to know if my design will work or not therefore I have already sent it for fabrication. Although, I solved the broken ground plane issue on the top layer and did the same as you asked. Let's see how it works in real life when I will receive my PCB's.
But the important thing is I am not using a Microstrip transmission line. I am using Coplaner waveguide transmission line(both top and bottom layers are ground). My calculations are based on that only.

Not going to partake in the entire discussion, just putting out there that you can use ceramic antennae as well. These take away at least some uncertainty from your design and are probably even more compact. Example:

http://www.vishay.com/chip-antenna/list/product-45218/

Yeah, that options is always available. I'll look into that if this thing doesn't works out.

I placed an order for 2 boards only so that I can test my design. Let see what happens. I'll update up guys after testing the design. Hopefully it will work.
 

Offline janekm

  • Supporter
  • ****
  • Posts: 419
  • Country: gb
Re: 2.4GHz PCB antenna design verification
« Reply #11 on: August 11, 2017, 12:20:45 AM »

Sorry, I didn't explain that very clearly. You are using what's called a "microstrip" transmission line between your radio chip and the antenna layout. This one depends on having a solid ground plane beneath it, otherwise the impedance will change, causing a reflection of the signal. You really want to try and keep the groundplane underneath the microstrip as solid as possible.

In general it's good practice for a 2-layer microwave PCB to keep the "bottom" layer as solid ground as is possible, for several reasons. If you need to have a trace cross the bottom ground layer, try and keep it short, and avoid having big "slots" in that ground plane (these can act as unintentional slot antennas). Another reason is that you don't want currents in the ground plane have to travel around the slot, leading to high frequency voltage offsets (again leading to EMC issues).

Some of the comments here about needing to get a university-level education in microwave circuit theory and antenna design to get a simple 2.4GHz transceiver working are a little over to top for my taste (smacks of elitism).
I don't have a formal background in any of that, but I have passed multiple products based on 2.4GHz transceivers that I designed following basic rules of thumb and public antenna designs through EMC and intentional emitter (CE & FCC) testing, always with a good margin. Both with UK and Chinese test labs. It's not actually that hard to pass the tests if you follow the transceiver vendor recommendations and good practice.

On the other hand some of the radio modules from China (like the little one with the 2x4 pin header posted in this thread) are terribly designed and will likely make your product fail testing (a module like that is pretty terrible from an EMC point of view)! I certainly wouldn't use them as an example of good practice.

Okay, Thank for the help. I was quite eager to know if my design will work or not therefore I have already sent it for fabrication. Although, I solved the broken ground plane issue on the top layer and did the same as you asked. Let's see how it works in real life when I will receive my PCB's.
But the important thing is I am not using a Microstrip transmission line. I am using Coplaner waveguide transmission line(both top and bottom layers are ground). My calculations are based on that only.
Ah, I missed that, but the same applies... the moment you have a break in the groundplane (now either next to or under the trace!) the impedance will change suddenly, and "bad things" happen. Mind you it's all a bit academic in your case... your "transmission line" is a tiny fraction of the wavelength long so none of this really matters much.

Quote
Not going to partake in the entire discussion, just putting out there that you can use ceramic antennae as well. These take away at least some uncertainty from your design and are probably even more compact. Example:

http://www.vishay.com/chip-antenna/list/product-45218/

Yeah, that options is always available. I'll look into that if this thing doesn't works out.

I placed an order for 2 boards only so that I can test my design. Let see what happens. I'll update up guys after testing the design. Hopefully it will work.

Those ceramic antennas are more compact, but in my experience perform worse than the larger PCB antennas. Partially because they tend to be designed to work with rather large ground planes next to them (for example a whole laptop for a dongle application), and with a smaller groundplane would need significant matching effort to make them work again. The PCB antennas for 2.4GHz are small enough in most applications and less trouble.
 

Offline bug13

  • Contributor
  • Posts: 41
  • Country: nz
Re: 2.4GHz PCB antenna design verification
« Reply #12 on: August 11, 2017, 10:00:18 AM »
I don't seem to see a matching network?
Zhuhua Wu
Electronic Engineering Student
 
The following users thanked this post: kony

Offline ASHU

  • Contributor
  • Posts: 32
Re: 2.4GHz PCB antenna design verification
« Reply #13 on: August 24, 2017, 05:59:53 PM »
I received my PCB's yesterday. I have to say that, it didn't worked out of the box. Had to tweak few settings and components as per the datasheet and finally it worked.   :clap:
My frequency was offset by approx 100KHz, after adjusted that setting, I am now getting as good of a performance as I was getting in pre build modules.  Range as well as performance, both, are Great.

Thanks a lot everyone for helping me out. :-+
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf