Wanted a Sanity Check before Ordering Custom PCB

[80k]

So I never created nor ordered a Custom PCB before, so I watched some YouTube videos of KiCad and attempted it. Considering how cheap it is these days to order a few prototype boards, I wanted to give it a try.

Just wanted to see if there was anything I was missing, with regard to getting a useable 2-layer PCB.
Here's the rundown:

• Wanted to make a 4ms Atoner in a BB size box with PCB mounted pots.
• I have verified the build (have built a couple myself), so confident with the circuit.
• Pretty comfortable with the ensuring my schematic in KiCad is accurate. I traced it several times and feel good about its accuracy.
• I set footprints for capacitors, resistors, diodes, sockets, wire holes, and trimpots using KiCad's library and measured everything very diligently. I feel confident with the hole sizes and footprints.
• I used a known footprint for the standard 16mm PCB mounted pots I will be using and double checked the measurements.
• After assigning footprints, I let KiCad (latest version 6) build PCB automatically into its ratnest. I then laid things out as best I could. Made traces on the top and bottom and vias where needed.
• I let KiCAD fix clean up traces, and then I ran the Design Rule Checker, and the only rules failing are soft warnings with some silkscreens clipped by soldering mask. But when exporting Gerber, I can see the option to delete those portions so believe this to be a non-issue.
• No other errors, and the import into JLCPCB seemed to work just fine.
• Besides the typical Gerber output, I also exported the drilling file and had it all included in the .zip file. I saw the rendered image on JLCPCB and can see the holes are there.

I also didn't see anything in the default JLCPCB options that I had to change. Any gotchas or things to look for?

Adding some images of the PCB layout as well as the 3D rendered images from KiCad.

Any advice or encouragement (or raised concerns) would be greatly appreciated! Thanks!

[GGBB]

Sounds like you've covered everything. But which DRC rules did you run - rules from JLPCB or something else? Rules/tolerances can vary between fabs. Some of the pad-trace clearances look extremely small to the point where in the diagram they look like they are touching - make sure you are testing with the tolerances that JLPCB allows.

Also - you should know that "16mm" pots are often larger in diameter - Alphas are typically 17mm. From the looks of your diagram you should be okay though.

My only suggestion would be to increase your trace widths - they look very small. Wider traces will handle soldering heat better, as well as  have less resistance and handle more current if they are supply traces.

[80k]

Thanks for taking a look!

So the default clearance/minimum's match JLCPCB's manufacturing capabilities. I may try to raise the minimum a bit and see which traces I can attempt to give a little more space. The trace widths are also bigger than JLCPCB's minimum, but I actually didn't think about it much. I will spend some time increasing trace widths and seeing if I can get do a slightly higher clearance minimum. Thanks again for the advice, really appreciate it!

[80k]

So per your advice, I went ahead and:

• Made ground and 9V+ traces at .635mm instead of the .25 minimum trace.
• Double checked other clearances and minimums at JLCPCB and confirm I am within their capabilities.
• Enforced a higher minimum clearance of .23mm instead of .20. Not much of a difference but gave me a chance to find the ones that were super close and improved upon it a bit.

I think I might go ahead and order it. At the price they are quoting, I feel like it's worth a try!

[antonis]

Definitely I'm not a skilled PCB design person but I think there are a few signal and supply paths routed in parallel..

[ElectricDruid]

The board and the parts layout looks ok, but the tracks are *superfine*. I would never use anything even close to the PCB fab's "minimum" settings, and I have my DRC set up for probably twice their limits in all cases. I'd want all those tracks and vias several times that size. To be fair, I mostly design stuff suitable for beginners to solder, so I'm deliberately making things extra-robust to avoid people lifting tracks by overheating and so on. My feeling is that those super-fine tracks are ok for high density digital logic boards and so on, but there shouldn't be any need for anything like that for any effects pedal we're likely to do!

I don't know how long it took you to get everything on there, but I'd say I normally lay out a board twice or three times. The first time almost everything goes on, but I get stuck with some tracks unroutable, or only routable in some hideous manner. So then I go back to the beginning and have a rethink about the component placement based on what I've learned doing it once through. If I'm lucky, the second time it all fits. Other times I repeat that process once more.

What's your scheme for what goes on which side? I usually put power and a ground plane on one side, and then route the majority of the signal traces on the other side. If it's a really complex design (and I don't think that it's just bad because my component placement is making it harder than it needs to be) I might consider putting mostly-vertical traces on one side and mostly-horizontal traces on the other.

One final thing I'd say is that I've always found layouts like that one where the pots don't leave enough space between their footprints to get a IC with passives on both sides to be the most awkward, so I feel for you. Have you thought about (or tried?) rotating the ICs 90 degrees and organising them in a line vertically down the centre?  IC 2 and 3 could got between the two rows of pots with plenty of space left and right for passives, and IC1 at the bottom similarly, maybe? (I don't know which pots connect to which ICs, so I'm just guessing based on your current layout).

[80k]

Thanks for the advice, really appreciate it! I placed an order last night since it's so cheap, but I don't mind doing another revision or using your advice for the next PCB.

I did use double JLCPCB's minimum for the trace widths... at 10mil's for everything except ground and power, for which I used 25mil's. But I did learn that the larger traces will make a more reliable board, in case components get changed out. I'm guessing this won't be too big a problem, since it's a pretty verified circuit, and I got a few trimpots where adjustment is needed.

I think your advice to complete start over at least once is a great one though. I think I got too invested in my initial placement, struggled a lot, and just made it work... but I think I could do a better job with a do-over.

Thanks again for the advice!

[GGBB]

What's your scheme for what goes on which side? I usually put power and a ground plane on one side, and then route the majority of the signal traces on the other side. If it's a really complex design (and I don't think that it's just bad because my component placement is making it harder than it needs to be) I might consider putting mostly-vertical traces on one side and mostly-horizontal traces on the other.

+1

I aim to have all traces on the bottom side (rarely achievable) or as many as possible so that the top layer ground plane is as contiguous as possible.

I also agree that the signal traces are still very thin IMO. I personally use .024" for power, .016" for signal, and a ground fill/plane for ground.

Clearances look much better overall now, but there are a couple of spots that look like they have errors (I don't use KiCad so I'm not sure how that is indicated, but the diagram has a number of little yellow arrowheads).

[80k]

+1

I aim to have all traces on the bottom side (rarely achievable) or as many as possible so that the top layer ground plane is as contiguous as possible.

I also agree that the signal traces are still very thin IMO. I personally use .024" for power, .016" for signal, and a ground fill/plane for ground.

Clearances look much better overall now, but there are a couple of spots that look like they have errors (I don't use KiCad so I'm not sure how that is indicated, but the diagram has a number of little yellow arrowheads).

Oh, those yellow arrowheads indicate areas where the potentiometer silkscreen overlaps with the pads. When exporting the gerber file, there is an option to delete those portions of the silkscreen that interfere, and according to the JLCPCB documentation, that setting is all that needs to be checked when exporting. I was pretty careful to look over every warning (yellow arrows) to be sure that it only pertains to this particular issue.

I think I should have increased from 0.010 to higher for the signal traces. I initially left it alone while comparing it to the schematic as it made the V+/Ground easier to differentiate, but I could have increased a lot of them before exporting the gerber. I do like KiCad and looking forward to making more PCB's, so these comments/ideas will help me with future PCB's.

[Kevin Mitchell]

Auto-route is the devil!

Kicad also has a design rule checker which is great for sifting out incomplete traces, conflicting placement and so on.
You can also set the design rules which is crucial for setting trace widths for specified nets - I always make the power traces thicker than signal. You probably wanted to do that before you cheated with auto-route.
(sorry, not sorry for the spite  )

Edit: Ahh I see you've already revised. My bad!

Also, I think you've chosen a footprint for 1/8w resistors. I mean 1/4 will fit given the wide spacing, they're just larger than the silkscreen. I'm not a fan of their resistor options and do my own for .1" spacing and no overlap.

[80k]

Oh I didn't use autoroute or anything. Laid it out myself, but probably didn't do that good a job  ... Not sure what the best size is for resistors, but I did measure the spacing used in some AionFX PCB's I had that fit my 1/4w resistors well and picked one that had the same spacing.

[bluebunny]

The board and the parts layout looks ok, but the tracks are *superfine*. I would never use anything even close to the PCB fab's "minimum" settings, and I have my DRC set up for probably twice their limits in all cases. I'd want all those tracks and vias several times that size. To be fair, I mostly design stuff suitable for beginners to solder, so I'm deliberately making things extra-robust to avoid people lifting tracks by overheating and so on. My feeling is that those super-fine tracks are ok for high density digital logic boards and so on, but there shouldn't be any need for anything like that for any effects pedal we're likely to do!

Bless you Tom - for your boards and for the wisdom.  If only everyone would take note!  I've had a few DIY boards that had tiny pads and were a b!tch to solder.  Funnily enough, all synth DIY stuff (nothing from this neck of the universe) and some of it from large-scale vendors.

[ElectricDruid]

Funnily enough, all synth DIY stuff (nothing from this neck of the universe) and some of it from large-scale vendors.

Yeah, I've had some Eurorack PCBs where the design objective was clearly "get as many features in there as possible!" and the PCB is crammed and the tracks and pads are tiny. Nightmare.