Is My PCB Good?

[masonfuses]

I am new to creating PCBs and I just designed this in Kicad. I am making it of the MAC2870 and the schematic I am building it off of is here https://www.analog.com/media/en/technical-documentation/data-sheets/max2870.pdf <-- page 23. Is there anything I need to edit here? I worry that the transmission line may be a bit small but i did the math for the copper board to be JESD51-7 and that is what the calculations added up to. Tell me what you think.

 

[jwin615]

Most here don't play in the MHz region.

 

[z2amiller]

I can take a crack. Is it good? Not yet (sorry but that's ok), and apologies if I sound a bit harsh:

First, it's really hard to give you a good review here. It's a low-DPI image and you have all of the fab text visible which makes it very messy and hard to read. Generally it's good to take a picture of the whole board with the fab and user graphic layers turned off, and individual pictures of the front and back copper. (And inner layers, too, if you have them, especially if they have traces).

That said, from what I can actually see (which isn't much):

* The hell is going on with all of the REF** items? Do you not have an actual schematic drawn that has assigned references? Use: Annotate Schematic on your schematic page if so. (lHonestly? t looks like AI drew this from a naked netlist it extracted from your reference schematic. Ask me how I know) You need to have reference designators ("refdes", like R12 or C9 or whatever) for a lot of stuff to work properly, and to be able to describe which component you're talking about.
* You need a ground plane. Both sides. You don't route ground as a separate net except in specific circumstances -- create a 'filled zone' and assign its net to GND, and press 'B' to fill it -- it will automatically connect all of the grounds. If there are RF-specific stuffs you can use keepouts.
* There's some weird routing - e.g. look at the traces going to CE, LE on your connector, they wiggle. Use the 'D' key to 'Drag' segments of traces around without erasing them and starting over -- sometimes you do have to start over, but often times you can drag things into straighter lines.
* Don't use right angles for traces if you can help it. (e.g. ground trace on bottom layer which shouldn't exist because it's a ground trace)
* Why does your trace cross layers right before it gets to REF** (see?!!)?
* You should use thicker power traces - at least 0.5mm. That's potentially overkill (there are calculators that tell you) but you don't necessarily want to shoot for the minimum that won't burn up unless you're engineering your way around a space constraint. Other traces could probably be thicker as well - no need to optimize for the thinnest thing that will fit.
* Put your board name and revision number on silkscreen. Sorry to tell you, you're going to have more than one version of this built, so better to grab the right one from the drawer.
* Round your corners (right click on the edge.cuts rectanlgle, shape modification -> filet edges -> 1mm). The 90 degree corners are sharp and the rounded corners look a lot more professional.
* How are you gonna mount this - will it just float in air somewhere suspended by connectors? (I mean, honestly there are worse plans for a small board like this). But if you're going to mount it anywhere, even just screwing it down to a piece of wood, you might want to have mounting holes.
(Mounting pad symbols on the schematic, make the holes whatever size you need)

 

[MattG]

Agree with @z2amiller, but also: it looks like the core component is a tiny QFN-style package, i.e. virtually impossible to reliably hand-solder? If so, that means you're probably looking at an assembly service (like JLCPCB). Combine that with "my first PCB" and it's a likely recipe for frustration and wasted money. Using JLCPCB's SMD assembly service isn't hard, but it's a whole 'nuther bag of small details that have to be carefully managed or the whole project might fail. And if you don't plan on an assembly service, hand-soldering ultra-tiny QFN packages is hard - I think they pretty much demand a precision reflow scheme.

I'd really suggest starting with a simple through-hole PCB design. Just pick a simple circuit, preferably a popular one (like a Tubscreamer or Timmy) and make your own PCB for it. Two-layer, unpopulated PCBs are super cheap, and through-hole makes it much easier to do the inevitable rework and debugging that comes with anyone's first PCB design.

 

[Locrian99]

Ever feel like an ai bot is farming your brain?

 

[z2amiller]

looks like the core component is a tiny QFN-style package,

Yeah - that, too. More importantly, it has a buried ground pad which means you can't solder this with an iron. You can kind-of-do-it with hot air though it means getting the component above its comfortable temperature (probably) since you have to get the component hot enough to melt solder underneath it _from the top_.

This is doable at home with a hotplate though, it's small enough. You don't really need a stencil, it's possible to just tin the pads, apply a bunch of flux, and let soldermask and surface tension work their magic. I'd really recommend a hotplate at home if you're doing SMD. You'd want to hotplate this first, before doing the through-hole stuff, which would make it stand proud of the hotplate on the pins and it wouldn't heat enough.

There are a couple of really great little hotplates - in particular the AlienTek HP-20 almost feels like it was made for guitar pedals. It has a heating surface of 100x60mm, which is about as large as you'd want to make a board for a 125B. It's basically the exact size I use for my designs that integrate the jacks at top and span all the way to the footswitch pins.

FWIW, I'm learning that AI actually can lay out boards and create reasonably human-readable schematics. I'm hacking at something not guitar-pedal-related -- making a dipole antenna for a ADS-B receiver, and Fable 5.1 has done an actually pretty good job with layout. I'd never have it create a guitar effect -- why automate my hobby -- this is a money sink for me, not a business. But what it DOES do well is verification - highly recommended to have an agent review your schematics and layouts before production.

I think like anything else it's garbage-in-garbage-out, you kind of have to know what you're doing first so you know what to ask for and know what to verify.