Submitted 1 week ago by eutampieri@feddit.it to electronics@discuss.tchncs.de
Hello, first time poster (and also no significant EE background, so bear with me).
After receiving a batch of bad USB C PD trigger boards, I decided that it would be better if I made some myself. The design is taken from the CH224K datasheet. However, I am not sure if a. the schematic is correct b. the PCB is well laid out (I really struggled to fit everything)
Here is the schematic, and here is the PCB. Both are in a Codeberg repo.
I’ll also jump in, mirroring some of what jeinzi said, and providing some of my own thoughts. I agree that both what you originally had, and what you have now should work.
Your schematic should read left-to-right with the flow of current. I don’t believe a wire is necessary, though I do see how it could be beneficial. The only thing I would change is flipping Q1 so that VOUT is on the right side of the schematic instead of being on the left as it is now. I had to do a double take to figure out what was going on there.
I also tend to prefer global labels, especially with a single page schematic like this, as they’re a little easier to read than the standard net labels.
On to layout, I’m a “Route Power, pour ground everywhere else” kinda guy. Remove islands, but I then via stitch all my grounds together. This is most useful for higher layer count boards and stuff dealing with RF. This shouldn’t see any of that, so it’s less of an issue. I rather dislike the setup with the 5 separate planes/pours on this board. I forked your repo and quickly threw together how I personally would route it, assuming I:
Hopefully that’s somewhat useful and doesn’t feel like I’m stomping on toes.
Some additional ancient knowledge. Try to avoid sharp angles when laying out traces. I see that you’ve got a lot of those, especially near the jumpers. The old wisdom is that acid from the etch can get stuck in the corner and slowly eat away at the trace. The honest reality is that this is not a problem anymore, but it is still generally recommended to avoid sharp corners. Especially when you’ve got the space to do so.
Re assembly. I think this is all doable by hand with a nice soldering iron and maybe a light pair of hobby magnifiers at worst. I strongly prefer “bevel” style tips. TS-BC2 for TS100/pinecil. You could also go with solder paste and either a hot air gun or a hot plate. If you get low melt solder paste (138C), you can even use an old clothing iron if you’ve got a way to hold it upright.
This is really scattered, so let me know if you’ve got any questions or if there’s anything I missed.
Wow, thanks! You’re not stepping on anyone’s toes. I’m a computer science guy that sometimes likes to dabble with electronics.
I haven’t looked at your PCB yet but I will considering merging this.
Also, how do I solder underneath the CH224K?
Ooh it does have a thermal pad…
In that case, I think you’re on the solder paste train. Get it in a syringe, and use a small lure lock dispensing needle/tip to put a dab (about the size of the pad) on each pad. If dabs are touching a little bit, its okay, but if your board is absolutely covered in paste, you’ll likely have problems.
Then with a pair of tweezers (I like the ifixit 45° ones), you can carefully position each component so its legs touch down into the paste.
Once all the components are on, you need to reflow it. A hot plate works, a clothing iron could work, you could even fill a junk/scrap pan (That will NEVER see food again) with sand and use the stove to heat the pan, removing it from the heat, and pulling the board with beefier tweezers once the paste has melted and wetted all the pads and pins.
Since solder paste is just a bunch of tiny metal balls suspended in flux, so have a fume extraction plan. When it all melts, there will be some smoke/fumes from the flux that travel upward. Try not to breathe those in. A little bit won’t kill you, but it is an occupational health hazard.
jeinzi@discuss.tchncs.de 1 week ago
tl;dr: I’m reasonably sure this will work as is.
The following comments involving my personal opinions might be most useful for more complex projects:
While I also try to isolate building blocks in my schematics, I think it’s sometimes beneficial to have some visible connections using wires. Your schematic isn’t very complex, but I still needed to jump around a bit to understand how current flows from the USB connection to the output. I would arrange the building blocks so that current flows from left to right and include one wire that starts at the USB jack, passes by the CH224K and its bypass cap, through the FET to the terminal block, so you can read the current flow like you would a line of text.
Layout:
Regarding both the schematic and layout: run the ERC/DRC and fix all errors and warnings. Most of it is noise, but hidden beneath that, serious issues can hide.
Another idea that might be out of scope for your project: You could add optional 5.1k pull-down resistors on the CC lines and a solder jumper from VBUS to VOUT. Then you could use the board even without the CH244K and the FET if you only need 5V.
eutampieri@feddit.it 1 week ago
I tried to implement all of your suggestions. Would you mind having a look now?
eutampieri@feddit.it 1 week ago
That’s an AMAZING comment, thank you so much!
Re: schematics. Will take this in consideration next time
Re: constraints and DRC. I haven’t done this yet because I’m really scared of the result (actually, I ran DRC and it gave me minor things). I didn’t want to invest too much time in something I didn’t know if it would work
Re: silkscreen. I placed designators there for space reasons, I will try and see if they would fit if smaller. Also, metadata in the silkscreen seems a good idea.
Re: U1. I was worried that moving the IC would mean rerouting everything. I noticed and thought “too bad”, but I will try this
Re: SMD handsoldering. I never tried this before, so I figured that for me 1206 would be a good place to start. 0603 would not be comfortable 😆, I envy your colleague
Re: C1. Will do!
Re: CC resistors. It’s a great idea!