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. 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-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.
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!
(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
You may want to check out the antenna on the nRF24L01 2.4GHz Transceiver.
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?
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.
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/
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.