Is it not possible to route it manually on two layers only?
What could be the downside of using freerouting plug for this board? Can it reallycause it not to work?
The downside to autorouting is errors like these.
It’s a relatively simple PCB, so sure it’s possible to do this properly on a 2 layer PCB. But each PCB is always a mix of goals. You seem to prioritize aesthetics (nice row of resistors) and compactness. That are two goals that make it much more difficult to do the routing properly. EMC compliance is probably not high on your list. It also looks like you made the classic beginners mistake of forgetting to reserve PCB area for the actual routing. And from there you glide into a grey area of what you consider a “working” pcb.
So do you recommend to make the board slightky bigger in order for being able to manually route?
At the end of the day im coming from the diy world of synthesizers made on stripboard so i can guess moving to pcb, even if route by a plugin, is much better the stripboard and wire routing(?)
You could either re-place all the components to make it easier to route, or rip up all the autoplaced traces and see if you can do a better job manually.
It’s always a mix of design goals, and compromises. I definitely recommend to ditch the auto router and route the PCB manually. (Autorouters can be a useful tool, but they are definitely not a magic tool that “simply does all the wiring” for you.) Footprint placement is a very important part of the PCB design, and learning what works (and what does not work) is something you only learn by experience.
When I design a PCB, I usually start without expectations of PCB size, and do the part placement and the routing for small sections of footprints that connect to each other. And from there I go to bigger sections, while also keeping an eye on secondary goals such as connector placement (acessibility) and switches / buttons (for example for a front panel) that have specific location requirements. But it’s an interactive process. On a PCB like this, it is not a good way to first fully do the footprint placement, and only then start routing the tracks.
Reserve some time to do this. It probably takes much more time then you would expect (My guess is 2 days of more just to route this PCB) It’s not just the routing, but from research to what are important factors for designing a “proper” PCB, to trying out things, then ripping them apart and doing things in a different way. It’s not the design process that is important here. It’s the experience in routing PCB’s that is the most valuable you will get out of it.
Shall I do copper pour on both top and bottom layers?
What does this gizmo do?
Does it use high frequencies? Does it have high-gain audio amplifiers?
No Higher then 10k-13k.
No high gain amplifier. only active low pass filter.
Here is the schematics:
pdf:
Untitled.pdf (133.4 KB)
6 oscillators from 40106 into low pass filter played by hands using copper pads
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 it’s 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 IC’s) and you should take proper care of it.
I really don’t 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 can’t 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.