Plz Critique My Layout

Stickman393

Stickman393

Well-known member
A'ite homies. I'm giving PCB layout a shot. This is my first, complete board layout.

@Chuck D. Bones posted these in the Boneyard: it's his PNP Servo Fuzz Face with his Simple Relay Bypass. Because good artists borrow, great artists steal.

ANYWHO...fuckin, brutalize me. Let me know what I did wrong. I NEED TO LEARN.

I haven't done the ground pours yet, or stupid doodles...this is just a basic layout.
Servo Fuzz Schematic.png


Servo fuzz PCb.png
 
Last edited:
The relay coil is connected directly to V+. If you want it to switch, you need to use the output signal from the 555.
And check the 555 connections, some stuff is connected incorrectly. Compare it against the standard bistable 555 circuit.
 
Huh. Correct. Whoops. Had adjusted the schematic a bit to account for different footprints. Didn't get everything back to normal.

Lemme fix that...
 
I'm by no means an expert, but here's some changes I'd make:

  1. Orient all the electrolytic caps the same direction. Makes verification easier and looks tidier. In this case it's natural to put negative down since two are already oriented that way and the other two won't be worse.
  2. The lower left transistor + R2/C10/R4 can be rotated as a unit and I think it would end up being tidier. Then you'd have the two transistors facing the same way, also useful for verification and looks tidier. You could then also pull in R17/R16 closer to the IC.
  3. I'd move the upper electrolytic cap to be on the blue trace you've already laid out.
  4. I believe you can line up R11/R13/C7/R8/R10 in a row, esp if you move the lower right capacitor down. A few would have to be flipped around.
  5. What width are the traces? They don't look right to me at a glance, there seem to be too many thick traces (more than I'd expect from the typical number of power traces) and the skinny traces are really skinny.
  6. Maybe it's just my eyes but the resistors look small. I'd expect the resistors to have pads with the same spacing as the DIP8 IC. This looks closer to a 1/8W than 1/4W? And the Diodes look huge by comparison. In my layouts the diodes are the same pad spacing as the resistors.
  7. It might be too late for you at this stage, but I'd also consider always orienting the ICs with pin 1 in the upper left. I always seem to mis-socket ICs and a consistent orientation makes it easier to catch.
  8. I'd consider rotating the 8-pin component (relay?) at the top. That would give some more space and I think you could line up R1/C4/R5/C5 with a vertical orientation. Pin 1 and 8 would also then have a more natural orientation, though it's hard for me to visualize the other pins. Pin3 would be an obnoxious route with that rotation but I think the rest would look better.
Here's a crude visualization of some of the above with magenta as new routes or rotations, and white as moved pieces:
1740222651479.png
 
Last edited:
^ love it!

Thanks! Gonna pore through that list and implement some changes.
rwl said:
  1. What width are the traces? They don't look right to me at a glance, there seem to be too many thick traces (more than I'd expect from the typical number of power traces) and the skinny traces are really skinny.
Click to expand...

10mils and 24 mils. I wasn't entirely sure where I needed to "end" the power rails. What's good practice here? Keep the rails wider until you get to the first load, then reduce trace width?

rwl said:
  1. Maybe it's just my eyes but the resistors look small. I'd expect the resistors to have pads with the same spacing as the DIP8 IC. This looks closer to a 1/8W than 1/4W? And the Diodes look huge by comparison. In my layouts the diodes are the same pad spacing as the resistors.
Click to expand...

I believe you're correct! Thanks, I had missed that bit.

*Monday edit* yup... those lil footprints totally fucked up my layout. Had to start from scratch.

Got a better layout now. Reduced everything on the power trace to 0.5mm, increased signal traces to 0.3mm.

Exporting from kicad is a PITA. Right now I'm printing to PDF, then importing to inkscape and exporting as a PNG.

woof.
 
Last edited:
If you're still open to comments, I will say some of your traces are WAY closer to some of the pins than I'm generally comfortable with. I would much rather have thinner traces spaced away from things than thicker traces jam packed everywhere. On typical designs I route things at 15mils (0.38mm) and on busier designs I'll go down to 12mils (0.3mm), on simple stuff I'll go as high as 20mils (0.51mm). I usually have the design rules set at a minimum 10mil space between copper, but when I route I try to keep it closer to 25mils just in case. I've had too many issues with crosstalk and noise in the past that it's better to play it safe.

Also, any particular reason you chose to do a ground trace instead of a copper pour?
 
MattG said:
When I just want an image of my PCB layout, I use my OS'es built-in screen capture tool.
Click to expand...
Fucckkkkk I feel dumb. Yeah. Thats easy.

vigilante398 said:
If you're still open to comments, I will say some of your traces are WAY closer to some of the pins than I'm generally comfortable with. I would much rather have thinner traces spaced away from things than thicker traces jam packed everywhere. On typical designs I route things at 15mils (0.38mm) and on busier designs I'll go down to 12mils (0.3mm), on simple stuff I'll go as high as 20mils (0.51mm). I usually have the design rules set at a minimum 10mil space between copper, but when I route I try to keep it closer to 25mils just in case. I've had too many issues with crosstalk and noise in the past that it's better to play it safe.

Also, any particular reason you chose to do a ground trace instead of a copper pour?
Click to expand...

Oh, it's gonna have a copper pour. This is pre-pour, to make it easier to see the traces. That makes sense in my mind for some reason.

Design rules...I'll have to take a look at that. Might help!

OK: updated layout. I ended up not keeping the polarity the same for all components: it just got too real with all the routing of traces and such.

I dunno. I ain't great at it yet, and I'm open to re-doing it.

Screenshot 2025-03-06 170034.png
Screenshot 2025-03-06 165601.png
 
Stickman393 said:
Fucckkkkk I feel dumb. Yeah. Thats easy.



Oh, it's gonna have a copper pour. This is pre-pour, to make it easier to see the traces. That makes sense in my mind for some reason.

Design rules...I'll have to take a look at that. Might help!

OK: updated layout. I ended up not keeping the polarity the same for all components: it just got too real with all the routing of traces and such.

I dunno. I ain't great at it yet, and I'm open to re-doing it.

View attachment 91827
View attachment 91828
Click to expand...
Dude, keep your damn traces away from your damn pads. I'm home now so I have more time to do stuff like this. Everything circled in orange is a spot where a trace is too close to a pad. It looks like you're literally too close for manufacturing, they won't be able to fabricate this without it shorting.

Also, what size is that via? Manufacturers will have a minimum size they can manufacture, and I know at JLC they have a minimum size then a minimum size they can do cheaply, i.e. if you do micro vias they charge you extra. On typical designs I do a 30mil annulus with a 16mil hole, on a really tight design I'll go down to 20mil/11mil, but I never go smaller than that on pedal stuff.

Untitled-3.png
 
Keep in mind, that's just the latest iteration from a few days ago. Before I read your comment.

I get what you mean: I'll look into setting up design rules to have kicad automatically keep a set distance from pads. This is just how kicad laid em out.

Good point on vias, I wasn't aware. I've been trying to avoid using them as much as possible for reasons I can only describe as "bewildered shame".
 
VIA icon-app.png

Not to derail your thread, but yeah, you've gotta watch out for those Via Rails...

1080.jpg
 
The spots I see with vias (not sure if I caught them all) could definitely be sorted thru rerouting instead. Just looking at C3/R4/R5 and R4/C10 (route it above the opamp right to C10)


is it Autorouted? It’s much more satisfying to jenga it all manually lol
 
Nostradoomus said:
The spots I see with vias (not sure if I caught them all) could definitely be sorted thru rerouting instead. Just looking at C3/R4/R5 and R4/C10 (route it above the opamp right to C10)


is it Autorouted? It’s much more satisfying to jenga it all manually lol
Click to expand...
Funny, I thought the exact same thing when I started fucking with it today. Vias are gone!

Nudged some stuff around. Couldn't find the setting for enforcing clearance from pads. How do I turn off auto routing? I just click click. Bang rocks together. Arg. Grunt grunt. Chuck fuzz board make bleep bloop.
 
Of course, you do you, but I like to manually route because I have an understanding of what components should be grouped together and where the audio path runs. I try to group logical components together (ie. all the power section, or all of a single gain stage) and give the audio path priority for clean, short traces.

Nathan has already mentioned traces and distance to pads, so I won't go there. But yeah..

Also want to give thought about practical assembly. C1 and C11 are pretty close to that pot, it'll be a pain to solder it in.
 
szukalski said:
Of course, you do you, but I like to manually route because I have an understanding of what components should be grouped together and where the audio path runs. I try to group logical components together (ie. all the power section, or all of a single gain stage) and give the audio path priority for clean, short traces.

Nathan has already mentioned traces and distance to pads, so I won't go there. But yeah..

Also want to give thought about practical assembly. C1 and C11 are pretty close to that pot, it'll be a pain to solder it in.
Click to expand...

manual routing is the true zen moment, followed by "why the fuck did I put that there?!?!" followed by more zen moments
 
From your latest iteration I think you need to take the design rules from whatever manufacturer you'll be going for and force them onto your design like @vigilante398 insisted on. The recommendation in general is placing what HAS to be at a certain spot, then work by groupings starting from the input.
 
You must log in or register to reply here.
Back
Top