here is my pcb design rules:
Anything to change?
Do I need to make different rules for GND and Vcc tracks? (make them wider?)
No. Use a single GND plane, and use tracks for the rest. If you want to take PCB design seriously, the video from Rick Hartley about achieving a proper GND is really worth itās two hours and 19 minutes.
No, that is not true. You are using CMOS logic 40106 has a rise time of around 50ns (@10V power supply, I see some 9V referenced in your schematic) and this inherently means your circuit has harmonic content to at least some 5MHz to 10MHz. Most of it is filtered quite soon to the audio frequency, but those high frequencies are present directly at the outputs, (And also on the power supply pins of those ICās) and you should take proper care of it.
I really donāt think it is possible to feet all of the signal routing and Vcc routing on one layer and only the ground on the other layer. If I need to have signal on both layer - I should try to no mix GND tracks with Vcc tracks?
I think it should be possible. I use 0603 resistors. Under 0603 I can go with only one track while you can go with plenty of tracks under your elements allowing to unravel the connections.
I spend about 80% of time on searching the element placement simplifying me the tracks that I have to then make.
Here is my example of 2 layer PCB with whole bottom being GND:
In VCC connection I used three 0R resistors to avoid having to go with tracks on bottom. The key conception was to go with VCC under the main microcontroller and spread it out radially from there to all other ICs.
You know how to do them . . . so this is not a KiCad question so is off topic for this forum . . . again.
I agree with you that OP need not help in KiCad use - he knows how to add zones.
But good routing is much more directly connected to the PCB designing (and so related to KiCad (not KiCad use, but only KiCad itself)) than any schematic question (that also happens here). I think we can accept to some level routing strategy discussions.
About your first post.
Error telling that connection of any pad is only one spoke while minimum is 2 you can avoid by changing minimum to 1 (Board Setup - Design Rules - Constraints). Single spoke connection is also connection so in most cases it is enough.
But Error telling that some pad is connected to zone isolated island canāt be ignored. You want all pads that you specify as connected to GND be connected together, but this error tells you that you have pad that is connected to GND zone part, but this part is island having no connection with whole zone. Such things happen when other tracks divide zone into separate parts. This never happens to me as I always use bottom layer only for GND. Even if you allow use this layer for as short as possible tracks needed to cross wires at top these small pieces of tracks will be only small holes in your GND zone and not divide it into separate islands.
But your elements having planty room under them allow to be used (by right positioning) to jump with signals over other signals.
For PCBs with THT elements typical in my opinion would be to connect everything at bottom and have GND at top. That way currents going in tracks have GND along them, but also currents going in for example resistors have GND as close to them as possible.
1 Like
I solved this problem by changing the problematic pads to solid as suggested. Will this be enough in my case?
That depends on the thickness of your copper, the power of your soldering iron, the melting point of your solder, how much heat your components can take.
This topic was automatically closed 6 hours after the last reply. New replies are no longer allowed.