Please advise reading materials on PCB layout (2 layers) on EMI (less noise generated by device) and EMC (able to work fine under external EM wave/field).
MCU core is not high speed but still want to do things properly. GPIO pins set to low current and slow speed. Has I2C (standard speed), UART (38400 bps) and non-frequent interrupts.
Many thanks
Hi @Dave1
I’m sorry, but this forum is about using Kicad, not reference books on electronic design.
You would probably get better results from forums such as EEVblog.
Depends on what circuit you are planning on laying out a PCB for.
In general good design is mostly in the circuit. For any high current switching circuits you want to have the minimum loop size for any changing current path.
As for general layout your best bet is to keep ALL I/O from to the board (including power) in one area of the board and bypass the signals right at the connection leaving/entering the board.
Else you will have to try google. All my application information is for “VERY” high speed circuits.
I hope links I provided long time ago are still valid:
For such 2 layer PCB the most important in my opinion is to have continuous GND at one side:
You can see such designed PCB here:
All vias you see are GND. I used there may be 3 0Rs to jump with VCC over signal lines without making a break in GND. As at each output line I use 47…100 ohm resistors (to limit current pulses taken by IC to change output state and I power practically each IC through ferryte bead in most cases I need not to add 0Rs to cross wires.
HI,
I disagree with this statement. I’m assuming you mean the ground side will be 100% copper with no traces or components. At the frequencies typically used for Arduino this adds little or no benefit for EMC. Not until you are working with “radio frequencies”. It may be beneficial to have ground under areas covering high switching currents.
I’ve found a “ground plane” under the area of the board where all inputs, outputs and power enter or leave the board. And have 0.1µf capacitors from this ground to the pin or solder point etc. This capacitor must be as close as possible to the pins. Any transient protection can come after this cap.
The goal here is to strip any RF/ESD from the signal before it gets into the circuitry.
I’ve never seen or used a ferrite bead to feed an IC. The most important practice is to put the bypass capacitor as close as the IC power - ground leads as possible.
My experience comes from designing boards that met Military EMC specifications for some boards and Automotive EMC specifications. I was lucky in my 2nd job, our company had a screen room and could perform all the required testing both conducted and emission/susceptibility. Being able to work in the screen room basically without additional cost allowed me to investigate solutions that may have not have been investigated at a $$$/hour testing lab. It was an immense learning opportunity for me.
I fill being no an expert here. I just base on articles from links I have given in my previous post,
I don’t know Arduino. I am designing PCBs to have as much EMC margin as possible. The question is not what frequency is on the Arduino lines but how fast are the slopes so what are the highest important harmonics. And I don’t know if signals going out of Arduino are filtered internally in any way or there are as fast as possible output at its pins.
Making GND having not breaks is not a big cost (in this example it was cost of 3 0Rs and their assembly) and gives you guarantee of having the best possible return path for all signals.
Capacitors are so obvious that out of discussion. But at these capacitors you still have RF pulses when IC is switching (capacitors have parasitic ESL). To eliminate a disturbance as close to the source as possible I connect this capacitor to whole PCB VCC via 1k ferrite bead. 1k means it has 1k impedance at 100MHz (while having about 0.3 ohm at DC). Ferrite beads differ from standard L in it that they don’t have tendency to resonate at higher frequency as their high impedance comes not from L but from losses (higher frequencies are converted internally into heat).
I seriously envy you.
I had only very limited (and always paid) access to such room. My experience is that my designs are enough good as till now each my device passed lab EMC tests for the first time.
For me these 3 0Rs is the cost for being secure from having to pay for tests twice.
Yes but there were many days I would have rather been somewhere else.
I understand you approach is very conservative. And you have the luxury of being able to layout your boards with all the circuitry on one side. Being in Aerospace I did not have the size luxury. Always size and weight were at a premium.
My original remarks were made with my mind on the need for your level of conservativism for what I believe are hobbyists.
If someone asks for EMI, EMC knowledge he is on the way from hobbyist to professional.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.