On a 2 layer PCB, is it better to have a ground plane and a power plane, or 2 ground planes and tracked power?
On a 2 layer board, typically:
The bottom is the ground plane and as few as possible vertical traces.
The top are the components and horizontal traces.
I donât mean vertical and horizontal literally but its best to try to keep bottom traces going in the same general direction.
When all done, review the ground plane looking for any places where the ground plane might be necked down causing a poor conduction path.
This is not an exact science. If you asked 3 very talented circuit designers to design a board, you would get 3 different designs.
In addition, Kicad (an most PCB programs) has set the default trace size and via size to the minimum producible by most vendors. You should not use these defaults unless you really really have to.
I bump my minimum trace to 0.35m and I double the via drill diameter. Also know vias are not as good a conductor as a trace. If you need power to go through multiple vias are desired.
1 Like
The GND plane is one of the most important parts of a PCB design.
There are plenty of designs which switch from 2 to 4 layers, just to improve the GND plane, and to reduce the amount of effort needed to route the PCB.
The GND plane does a few things.
Firs it (usually) is the voltage reference for all signals of all ICâs.
Secondly, for all signal content of frequencies above a few kHz, the path of least impedance for all signals is not the lowest resistance, but the lowest inductance. And the inductance is (grossly) defined by the loop area between a signal line, and itâs return path. With a continuous GND plane the return path of the current will be directly below the signal track. This phenomenon gets notiicable at a few kHz, and for 50kHz upward the return path will be very close to the signal path indeed. (If possible).
Without a continuous GND path, the return current can not be close to the current in the track (No high voltage generators here, current always goes in circles for practical PCBâs), and the increased loop area will radiate outwards, and reduce signal integrity, and cause EMC problems.
There is generally no need to make power planes for the power supplies. That is what local decoupling is for. For logic level PCBâs you need a decent track width for the power to reduce voltage droop, but all currents above a few kHz should be delivered by you decoupling capacitors, and therefore itâs mostly the DC resistance that counts for the power tracks.
That was the short and simple version.
An interesting video about this subject from our competitors below.
Itâs two hours long, but if youâre interested in this part of PCB design, it is worth watching.
3 Likes
Attention to detail like Rick Hartley is likely of little concern for most hobbyists. I donât know what you plan to design but things like driving LEDs, relays etc are considered âlow speedâ for the types of issues Rich is dealing with.
So for now I suggest you stay with the basics. If you feel you might need a more esoteric design post your schematic or at least describe what you want to do.
Hi, JohnRob
Just to say that I have seen a very simple design which was screwed up by bad layout. This power supply had a mains frequency transformer, bridge rectifier, 1 large and 1 small electrolytic capacitor, and 7805 type 3 terminal regulator. I am not sure what are the bounds for âhobbyistsâ; I started out as one. But anyway this rudimentary power supply had improperly high 2x mains frequency output ripple due simply to bad routing of a ground trace. I think that diving into and understanding these details is part of what makes this stuff interesting. âThe devil is in the details.â
1 Like
Is there a prefered way to join bits of plane that end up as islands?
I have assumed I just drop vias in to join the front and back planes as there are rarely isolated bits of plane exactly over each other.
Iâm not doing anything particularly high frequency so I can pretty much drop the vias in where ever, but whatâs best practice?
It comes down to understanding the current flows and identifying what is important. Basically the pcb presents a set of components which will introduce resistance, inductance, and capacitance. You need to understand how to design to design the pcb so that these stray impedances do not cause problems with your circuit. We may be able to discuss specifics if you were willing to present your circuit diagram and perhaps describe it in detail. But giving away those details may or may not be something you want to do. If you do not want to do that, then you need to study the available generalized recommendations and figure out how to apply them to your board.
It is possible that your design may be relatively immune to effects of variation of normal pcb layout. My earlier point: It is easy to assume that a design is immune to normal reasonable layout variations ** but that assumption might turn out to be wrong.
**By " normal reasonable layout variations" I mean that the designer is not for example trying to lay out the board as badly as possible, perhaps to prove a point.
I agree 100%. But at the same timeâŚ
In my younger days worked for boss who had a saying that compared a person to an opamp. " If you overload the input you get nothing out".
Maybe in this case the best advice is to read the application details for the component you are using. I know of any way I could write a post that would impart my (by now intuition) designing boards.
First ask, are there any current carrying parts connected to the island?
If so try to move thing around to allow the Isolated island to become a peninsula with a fairly wide width.
If not try moving things but not as aggressively as above.
Else connect it to either gnd or +V. NEVER connect it to a signal.
'__________________________________________________________________________
As I thought a little more about the questions it struck me the first step is to understand the circuit requirements. So the place to start is to list the critical requirements of the circuit.
I couldnât even begin to provide a sufficient list of critical circuit parameters but a few that come to mind are:
- Know how sensitive your signals are. Keep power components away from low level analog components.
- Capacitors: 90%** of the time they are to reduce unwanted high frequencies. The must physically and electrically close to the components whey are protecting.
** other 10% are large power supply capacitors should be kept with the power generating circuit. - Vias are not good for power. Making them larger than the default and adding multiple parallel vias helps.
That is a good one. But I think the op amp is much more linear before you reach that point.
2 Likes
âHigh frequencyâ in this case really means signal rise time, not repetition rate. For example, a 1 Hz square wave with a 2 ns rise time contains the same harmonics as a 200 MHz square wave. That includes all the related effects such as ringing.
Itâs often sufficient to slow the signal rise time to avoid problems like these. But ignoring the problems doesnât make them go away.
1 Like
As I said before, the GND plane is usually regarded as the return path for all currents, and above a few kHz signal content (Mainly defined by rise time, as RRpollack correctly added) If you keep this in mind, then do a sweep through your project, highlight each signal track, and then consider the return path for each signal, and place stitching viaâs to reduce the loop area.
But for a pretty big part, itâs also what you consider good enough for yourself. Itâs much easier to make a PCB that works good enough for yourself, compared to a PCB that has tho pass EMC tests.
Apart from that, there are many areaâs which may need special care. A classical example is the PCB layout of audio power amplifiers. This is a combination of very low level signals (Standard audio input is about 1.5V, but you want 120dB (or even much more, if you consider the volume potentiometer) of dynamic range on that signal, and which also has high currents and high voltage swings, and nearby big transformers with leaking magnetic fields. Many engineers have spent countless hours to get their design right, even though those amplifiers usually have a cutoff frequency of around 100kHz or lower.
In my opinion, 2 GND planes/filled zones.
It is my opinion that an outer board layer with a filled zone with power is just asking to let the smoke out in the future. Every zone connection to power will have a small area missing the solder mask.
It has been my expeience that Murphy and his Law has something to do with this.
1)Any apparently clean electrical connection can fail to connect at the most inconvient point in time.
2)Any apparently dirty/insulated connection will fail to insulate at the most inconvient point in time and let the magic smoke out of the device.
Although 2 may seem the obvious easiest âhobby routeâ it is not. There are many great youtube videos on pcb layup that are worth watching and how it works. Best is 4 as its easier routing and far better for emc and other issues. If you are not making the pcb yourself the cost is also no stumbling point. Its a fallacy that 2 is better.
I would like to ask for clarification. Two layers? You probably mean a four layer board with two internal layers that you might make ground or power and then two outer layers for traces to connect components.
Please clarify.
If you really mean only two conductive layers (front and back only), the answer will be quite different.
Do you intend to use through hole components or SMT or a mix?
Assume two layers top and bottom. For ease of trouble shooting you want all components and most traces on top. Make ground the bottom. Make the bottom almost solid ground with only small islands of penetration for signals and power to jump one another. All connectors with ground shells should be well connected to the ground and up on the top layer too.
My personal opinion and product design opinion.
Iâve used 2 layer boards for 80% of my designs. We only went to 4 layers when we couldnât connect everything on a 2 layer board.
EMC was handled by careful layout. Iâve designed for both military and automotive. It seemed to me the automotive (which came after the military) EMC was more stringent, or at least had some more significant testing. One was bulk current injection.
Weâve always passed and our designs were usually in plastic cases with one side aluminum.
For a hobbyist for a new design I believe starting off with 2 layers is wise. Simpler, easier to troubleshoot and/or modify and less chance of design errors.
One tip to a new hobby designer: Never connect two pins of an IC under the IC. If you find you need to change the connections you cannot get to the trace without removing the component.
2 Likes
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.