Pcb Review Request - Page 1
Forum section: electronics / projects

author: Denis123
author_rank: Newbie
timestamp: August 31, 2025, 02:40:01 pm
content: Hi! I just made my first pcb wich is a bike speedometer and im worried about issues with my ground planes. The red and blue fills are the gnd planes. My board has a rpi pico, a 74hc595, a 2x7 segments display, a BQ24074RGTR and a voltage booster module. I just need a quick review of the layout of my pcb. Can someone help?

author: tooki
author_rank: Super Contributor
timestamp: August 31, 2025, 07:38:49 pm
content: Could you please make higher-resolution screenshots (or export PDFs) of the schematic and board? They’re just blurry enough to be annoying and strained to read.Also, on schematics, never run connections through component symbols. Always, always go around. (It even looks like you have components overlapping? Please fix that.)

author: mariush
author_rank: Super Contributor
timestamp: August 31, 2025, 08:51:13 pm
content: If it's not obvious what's bad ...From top to bottom ... Rotate the buzzer so that the negative is at the bottom and the positive is at the top.You can either move it to about where C9 is located and move C9 to the left of the buzzer.If you decide to keep your design like this with the shift register, you could take the two traces going to the display and route them to the right a bit, then under the buzzer and then towards the display. With the traces going straight up or a bit to the right, up and then towards the display, you now have space right above the 3rd through hole to put the resistor and the transistor there, instead of routing that trace under the headers.Change your transistor to some surface mount version. S8050/SS8050 are super cheap :https://www.lcsc.com/search?q=S8050&s_z=n_S8050If you keep the shift register, it's fairly obvious that the resistors and the traces use a huge amount of space.Use resistor arrays to make it shorter, you can get 4 or 8 resistor arrays where each resistor is about the size of a 0603 resistor, so still easy to solder by hand.example 4 x 270 ohm in 1206 package : TC164-JR-07270RLhttps://www.lcsc.com/product-detail/C872319.htmland in smaller 0805 package :https://www.lcsc.com/product-detail/C728775.html8 x 220 ohm in 1060 package (equivalent of 8 0402 resistors) :https://www.lcsc.com/product-detail/C874540.htmlYou can place them either directly above the output pins of the shift register, or you could rotate them clockwise and put them near the display.I was saying if you keep the shift register, because it would make more sense to just use a led driver (but you'll need to use displays with 8 anodes and 2 cathodes).For example, you could just have a GN1650 chip :https://www.lcsc.com/product-detail/C427456.html/ TM1650 :https://www.lcsc.com/product-detail/C22374376.htmlDatasheet is in chinese but you can use google translate to translate it. Skip all the stuff about readying buttons, all you need to know is that it can control up to 4 digits, up to 8 segments (8 anodes, it connects one cathode at a time to ground, loops through the digits)You don't need resistors, the driver limits the current on each segment. You could use only 2 cathodes, or you could connect each digit to 2 cathodes, and send the driver duplicated information every time (for example if you want to display "12", you send "1122" or "1212" to the driver.OR, you could use a 16 channel shift register led driver and use two separate digits with one anode and 8 cathodes eachSee for example SM1630S -https://www.lcsc.com/product-detail/C2830324.html- or TM5020A :https://www.lcsc.com/product-detail/C2980109.html(same pinout for both)One resistor sets the current for all channels, then you just shift in 16 bits and hit the latch to update the two digits.You could probably move J4 to the left side of the board, above the led, then you'll have room to potentially rotate the header counter clockwise and keep all those traces go straight to the left and into the header pins, and your two thick traces won't have to cross to the bottom layer, you can route them above the header if needed.

author: Bud
author_rank: Super Contributor
timestamp: September 01, 2025, 12:26:35 am
content: This 'schematic' is unreadable. Was it it some stupid AI that created it for you? In any case, you should start with what user tooki asked you to do, before getting to the ground plane. Because first it needs to be understood how the circuit is supposed to work.

author: ChipSniffer
author_rank: Newbie
timestamp: September 03, 2025, 03:20:53 am
content: Nice first attempt! From what I can see, the layout is generally okay for a beginner board, but there are a few things you might want to clean up. Your ground planes look a bit fragmented — there are several areas where the pours are cut up by traces, which could create ground loops or increase noise on your speedometer signals. Try to keep one solid continuous ground plane if possible, and route signal traces on the opposite layer.Also, check the clearance around your via stitching — a few look very close to pads, which could cause solder bridges. If your voltage booster module is a switching regulator, it’s a good idea to keep the input and output capacitors as close as possible to the IC and minimize the high-current loop area. That will help reduce switching noise, which is important if you’re measuring signals from a hall sensor or wheel magnet.One last small point: avoid running traces diagonally through component pads (like it looks near your 74HC595). Rerouting around components keeps assembly cleaner and avoids potential shorts.Overall, it’s a great start — a few layout tweaks will make it much more robust electrically.

author: CaptainBucko
author_rank: Regular Contributor
timestamp: September 03, 2025, 03:47:26 am
content: I would add some test point loops to the critical nets so you can easily probe them