Bring out yer Diptrace

[pingpongcomputer]

Gotcha. I use V- or DC- for that pad on my schematics. It might be worth changing the name because the negative connection is 0v, not -9v.

Feeling real dumb, -9V on one side and +9V on the other wouldn't be a 9V power supply. I wasn't thinking, just trying to fit things from the supply pins category of the rullywow library into the schematic for the pads I knew I needed for connections on the board. Many thanks, I also forgot I had one of your schematics to use for reference, that will be very helpful. I obviously need to do some more research.

Runoffgroove is doing this in several of their circuits as well. The DC check suggested above is a good idea, but if you're not after the clipping character of the LEDs, I wouldn't recommend moving them. It also might be worth just keeping them in case you want to put a booster or something ahead of this circuit that might change the character.

That part of the circuit is modified from part of a ROG circuit, that's why it looks familiar, and I plan to keep the clipping sections for exactly that reason, since I'm a fan of gain stacking.

Thanks very much @PedalBuilder and @Silver Blues , I'll be begging for help again soon with a pcb layout review and will hopefully include all relevant information.

 

[pingpongcomputer]

Ok, well I got sick and the circuit went through about 10 more iterations, but I got way better at diptrace schematic drawing, and schematics in general. Here's my first PCB attempt, from what I've read I think I should do a copper pour on the top layer too, but I left it off here so you can see all the traces. Almost everything is on the top layer except for a few stretches that couldn't be made and the ground pour. Hopefully the color scheme is high contrast enough for everything to be visible. Any critiques are appreciated.
Edit: I already want to change the transistor labels to Q1, Q2, etc rather than the type.

 

[Brett]

Any critiques are appreciated.

Can you take a snap shot of the board showing your ref des and share it here?

I see at least one trace that can be shortened significantly but telling you it's the 470pF capacitor does less for you than telling you it's C3.

Your 1µF capacitor footprint at the top is a bit too small if you're planning on using a film box cap.

Make sure you use thermal reliefs on your ground pours, otherwise, you'll struggle soldering them.

Your round solder pads at the bottom could probably use an increase to the annular width, otherwise, they may be difficult to solder.

This is just on a quick glance. Share the ref des when you get a chance so we can take a look.

 

[pingpongcomputer]

Can you take a snap shot of the board showing your ref des and share it here?

I see at least one trace that can be shortened significantly but telling you it's the 470pF capacitor does less for you than telling you it's C3.

Your 1µF capacitor footprint at the top is a bit too small if you're planning on using a film box cap.

Make sure you use thermal reliefs on your ground pours, otherwise, you'll struggle soldering them.

Your round solder pads at the bottom could probably use an increase to the annular width, otherwise, they may be difficult to solder.

This is just on a quick glance. Share the ref des when you get a chance so we can take a look.

Thanks very much, I think I fixed everything you outlined except didn't see the path to be shortened, but I'm still heavily under the influence of dayquil. I used 4 spoke thermals without doing any research, I'm guessing there are some sort of guidelines for what to use when if I do a little googling. I just copied the width of the pads for the resistors for the 3dpt connection solder pads, with 1.1mm holes, now that I'm looking at it maybe I want to bump up the pad width a little more.
Here's the revised layout with refdes:

 

[Brett]

Check the junction net at C4 and Q4’s base.

Edit: not C4, C17 and Q4’s base.

 

[derevaun]

I'd check the C17 traces against the schematic--if it had you follow a ratsnest line, there could be an incorrect connection.

The G2 pad takes a long and convoluted path to the ground pad at the top, including passing through R1's thermals. I like to evaluate the ground pour after every trace I put on that layer, making sure it's a pretty solid path to the primary ground pin. Vias can help a lot with keeping traces short on a pour layer.

 

[pingpongcomputer]

Check the junction net at C4 and Q4 base.

I'd check the C17 traces against the schematic--if it had you follow a ratsnest line, there could be an incorrect connection.

The G2 pad takes a long and convoluted path to the ground pad at the top, including passing through R1's thermals. I like to evaluate the ground pour after every trace I put on that layer, making sure it's a pretty solid path to the primary ground pin. Vias can help a lot with keeping traces short on a pour layer.

Thank you! Man, I made one last minute addition and two part swaps on the schematic before converting it to PCB and totally wrecked my connections in the boost circuit. Still passed all the verifications because they were connected to something, but not the right things. I would not have caught that looking at the PCB. I'm going to stop now and re-check everything tomorrow, thanks for saving me from wasting my first trial run.

 

[Brett]

Check R3 when you take a look tomorrow. That one’s got something weird going on.

 

[pingpongcomputer]

Check R3 when you take a look tomorrow. That one’s got something weird going on.

yep, that was part of the tornado of destruction I made adding one resistor and swapping 2 patterns.

 

[szukalski]

@pingpongcomputer your audio path should be as short as practically possible and avoid crossing over itself where you can.

Your input and output traces overlap each other, albeit on different layers. This could bring oscillation, especially in higher gain applications.

 

[Brett]

I've designed and verified several boards successfully, but I have no formal education in PCB design, so take my suggestions at face value.

Referencing this post:

Check the junction net at C17 and Q4’s base.

If your nets are connected correctly per the schematic, this trace is much longer than it needs to be:


To piggyback on what @derevaun said, your ground pour isn't ideal for the G2 pad. You also need to be sure to remove copper islands, otherwise, you may inadvertently create more noise in your circuit. Areas in green are connected. The uncolored portions are islands:


The component placement could be optimized in several cases. Like @szukalski mentioned, you want to keep traces as short as possible and keep traces carrying your input as far away from traces carrying output as possible. Even on opposite sides of the board, if in/out traces run parallel in close proximity, you're inviting potential problems.

 

[pingpongcomputer]

Thanks for the help everyone, I've been watching youtube diptrace tutorials but they haven't been audio focused, just getting an assembly together. I learned how to use vias this morning and I think I've cleaned things up pretty well, but I'm going to try to optimize component placement some more for a shorter audio path. Grounds look better though and I think all the big islands are gone, just a little one near the traces between trim2 and the density spst.

 

[Brett]

Grounds look better though and I think all the big islands are gone

Indeed, the ground pours do look better, however, you may want to increase thermal spoke count. Take a look at the ground pad "G" on the bottom left. There's only one spoke connecting the pad. Many others only have two. Two is acceptable if you're not dealing with increased currents, but I personally like to have at least three, preferably four. You should be able to select a setting that removes copper islands in your ground pour.

I learned how to use vias this morning and I think I've cleaned things up pretty well

Vias can make things easier and are necessary at times, but they shouldn't be used as a crutch for a subpar layout.

• Take a look under R13. You can just route that trace on the bottom layer and skip the vias.
• Same with the trace under C2. The trace that's going to "RE" pad on the bottom right can just be routed around pin 1 of the BLEND pot and CLR2, no via necessary.
• The trace connecting R6 can be brought to the top layer and lose one via there.
• I'd also increase your trace width for any traces carrying power. Some of yours look a little thin.
• Also, a reminder, your footprint for C7 and C20 are a bit small if you're planning on using box film caps.

These are just a couple things I noticed at a quick glance. Not to sound too critical, but there's still a lot of room for improvement, and I'd start by optimizing the component placement.

 

[pingpongcomputer]

Indeed, the ground pours do look better, however, you may want to increase thermal spoke count. Take a look at the ground pad "G" on the bottom left. There's only one spoke connecting the pad. Many others only have two. Two is acceptable if you're not dealing with increased currents, but I personally like to have at least three, preferably four. You should be able to select a setting that removes copper islands in your ground pour.


Vias can make things easier and are necessary at times, but they shouldn't be used as a crutch for a subpar layout.

• Take a look under R13. You can just route that trace on the bottom layer and skip the vias.
• Same with the trace under C2. The trace that's going to "RE" pad on the bottom right can just be routed around pin 1 of the BLEND pot and CLR2, no via necessary.
• The trace connecting R6 can be brought to the top layer and lose one via there.
• I'd also increase your trace width for any traces carrying power. Some of yours look a little thin.
• Also, a reminder, your footprint for C7 and C20 are a bit small if you're planning on using box film caps.

These are just a couple things I noticed at a quick glance. Not to sound too critical, but there's still a lot of room for improvement, and I'd start by optimizing the component placement.

I'm grateful for the help and I'll take any criticism and suggestion. I wasn't trying to sound like I had it all figured out, just to say how well everything cleaned up after the suggestions, reading it back I can see how it comes off cocky though, I do not feel that way and know that I'm far from being good at this. I accidentally left the routing for the ground net on the bottom layer and was jumping over it with vias which was making things unnecessarily complicated. Those are gone now and I'm re-doing pretty much everything for better component placement. It's a little sad to scrap most of the work, but I learned a bunch a long the way. Taking note of everything else to incorporate in the new layout, thank you.

 

[derevaun]

One thing I like to do is save a copy and just unroute the whole thing and redo it. I always find a few ways to simplify. Or even (gasp) run the auto-router just to see what it comes up with. Usually it reveals where moving a part could lead to simpler routing.

I also like to keep in mind that while there's real satisfaction to designing an elegant layout, it's OK to just be done with a wild convolution that's still gonna sound just fine as a dirt box. So prioritizing parallel traces and squeezed current paths, e.g., gets me there faster. Even long traces on the board (notwithstanding interference) are gonna be shorter than some offboard wires. This shit is supposed to be fun--if it isn't anymore, I'm back to board shopping.

 

[finebyfine]

continuing to throw an opamp octave up in front of every circuit. this is into a frantone creampuff into the grindcorefx ultrastoner tone stack with a black tiger boost tacked onto the end

 

[Brett]

continuing to throw an opamp octave up...

One of the 2M2 resistors in the bottom left has the value facing the wrong direction. Not sure if you noticed, but it'd drive me nuts if I missed that before sending it off for fabrication.

 

[Brett]

A follow-up to my previous post, did you intend on using RED LED clippers on OA1/OA2 of the 4558? If so, your board has DO-35/DO-41 footprints in those positions. Not sure if that was intentional. Your board looks great if I didn't mention that before.

 

[finebyfine]

One of the 2M2 resistors in the bottom left has the value facing the wrong direction. Not sure if you noticed, but it'd drive me nuts if I missed that before sending it off for fabrication.

Great catch, I caught it a little bit after I posted the screenshot

A follow-up to my previous post, did you intend on using RED LED clippers on OA1/OA2 of the 4558? If so, your board has DO-35/DO-41 footprints in those positions. Not sure if that was intentional. Your board looks great if I didn't mention that before.

I have a handful of 1.5mm axial LEDs that work in that footprint but I also figured I'd try other do-35/41 clippers

 

[Feral Feline]

Cool logo on the PCB, @finebyfine, and the circuit is interesting too.

Might have to breadboard a CreamPuff>UltraStonerTS>TigerBoost.