Electronics > RF, Microwave, Ham Radio
First RF PCB Design
x4ce:
Hi,
I am an amateur in the field of PCB design and my experience includes multiple PCBs design of basic digital electronics and STM microcontrollers etc. I have got them manufactured by JLCPCB and they worked, successfully. This is my first basic RF PCB designed in KiCad and requires some guidelines before I go for assembly etc.
The frequency signals range from 250 to 500MHz.
What I know and have done so far:
The lengths of traces carrying the high-frequency signals should be shorter than 1/10 of the wavelength of the highest frequency taking into account the propagation delay due to PCB.
The traces for high-frequency signals should possibly remain straight or should have a radius of curvature.
The width of high-frequency signals should be 3mm in order to match the impedance of 50ohm for PCB of 1.6mm thickness & FR 4.6.[/li][/list]
The guidelines required are:
1. Is the ground fill zone/ place fine on the top layer with RF signals?
2. If ground fill/ plane is not required on the top layer then I need to put via holes for ground pads. Any criteria for this? There should be at least 2 via holes? Distance between them etc.?
3. The pads etc. do no match the trace width (0.3mm), would they affect the impedance matching, and, if so, what is the solution?
4. Should I place a guard ring around the whole PCB or between the input and output antennas?[/li][/list]
I have attached the initial PCB design with component detail on the silk screen for ready reference.
I will be grateful if someone could guide me.
Regards
Shahid
TheUnnamedNewbie:
I think you should start with sharing the schematic. It is too much work for me to bother looking at a PCB and try to figure out what traces are doing what.
--- Quote from: x4ce on October 12, 2022, 07:23:52 am ---
The frequency signals range from 250 to 500MHz.
--- End quote ---
This isn't too high yet.
--- Quote from: x4ce on October 12, 2022, 07:23:52 am ---What I know and have done so far:
The lengths of traces carrying the high-frequency signals should be shorter than 1/10 of the wavelength of the highest frequency taking into account the propagation delay due to PCB.
--- End quote ---
This is a common rule of thumb, but the main thing is not that they should be shorter, rather that if they become longer, you should start taking the line impedance into account.
--- Quote from: x4ce on October 12, 2022, 07:23:52 am ---The traces for high-frequency signals should possibly remain straight or should have a radius of curvature.
--- End quote ---
At 500 MHz, this doesn't really matter too much.
--- Quote from: x4ce on October 12, 2022, 07:23:52 am ---The width of high-frequency signals should be 3mm in order to match the impedance of 50ohm for PCB of 1.6mm thickness & FR 4.6.
--- End quote ---
That is quite a wide trace. I would consider going for a 4 layer PCB for this kind of design, as routing without disturbing your return currents will be challenging at best on a 2-layer PCB. A 4 layer PCB will also reduce your 50 ohm trace width significantly and as a result make the entire routing process more manageable.
Most of the issues you talk about in your questions are minor, likely even insignificant, at 500 MHz, unless you are doing ultra-high-precision measurements or super sensitive measurements (at which point you should stop using rules of thumb anyways and switch to using electromagnetic simulators).
500 MHz has a wavelength of like 60 cm in free space, so unless your PCB is massive, and don't break your return currents, things will be fine.
x4ce:
Thanks for the reply and guidance.
I have shared the schematic for your ready reference.
As far as the trace width is concerned, it was a typing mistake and the correct trace width is 0.3mm.
Please if you could further guide for the following concerns:
The guidelines required are:
1. Is the ground fill zone/ place fine on the top layer with RF signals?
2. If ground fill/ plane is not required on the top layer then I need to put via holes for ground pads. Any criteria for this? There should be at least 2 via holes? Distance between them etc.?
3. The pads etc. do no match the trace width (0.3mm), would they affect the impedance matching, and, if so, what is the solution?
4. Should I place a guard ring around the whole PCB or between the input and output antennas?
Thanks
T3sl4co1l:
There's no ground vias, and only a couple thru-pins connecting the layers? Yipe!
Roughly speaking, a via per pad, plus vias flanking especially longer traces, plus vias scattered around evenly (in a grid, error diffusion, whatever you like) will greatly improve things.
Tim
kml183:
Hi! Cool design! I am a RF newbie as well.
Like the TheUnnamedNewbie said, you might want to use a 4 layer pcb stack up like the JLC7628 or JLC3313. Those are the two main controlled impedance stackups that JLCPCB offers as well.
--- Quote from: x4ce on October 12, 2022, 08:18:30 am ---
As far as the trace width is concerned, it was a typing mistake and the correct trace width is 0.3mm.
--- End quote ---
You are also creating a co-planar strip line with the top copper pour. If you want to do this, (as I understand there are some benefits like lower trace losses for higher power), you need to make sure the spacing between the trace and copper pour is correct as well. See the attached image for some calculations with the KiCad transline calculator.
To answer the rest of your questions.
2. With RF stitching vias there seems to be many rules of thumbs that people use. The one that I have been using is the grid spacing should be at maximum 1/6 of your max wavelength which for you is 5 cm (c / 500Mhz / 12). The other one that I have seen for higher speed designs ( > 1G ) takes into account the velocity factor which is 1 / (e_r ^ -2 ). E_r is the effective permittivity of your dialectic (4.6 for FR4) so something like (velocity_factor * c / 500Mhz / 12). Either way if you have vias spaced closer together you are fine. :-//
3. For your max frequency it won't make much of a difference. So I wouldn't worry about it. What you can do is use traces of varying sizes to create a gradient from your larger pads down to the 0.3mm trace width.
4. You can if you want to. It won't make much of a difference because your PCB is only using 1 signal type. Guard rings are more useful for mixed signal boards to combat interference between the signals. I would just make sure that my vias stitching the GND planes together extend close to the end of the PCB.
Navigation
[0] Message Index
[#] Next page
Go to full version