My POV fidget spinner project / Check my PCB please - Page 1
Forum section: electronics / projects

author: buck converter
author_rank: Regular Contributor
timestamp: May 23, 2017, 08:54:23 pm
content: so i thought I would make myself a fidget spinner that uses 5 leds to display stuff. It is controlled by an attiny84a, has buttons to change the mode and even a hall sensor so it can sense speed and direction. powered by a 20 mm coin cell. I am just hobbyist in high school and will etch these boards at home. I will only make a few, some to sell at school. this is my first time working with SMT, so i limited myself to 0805 and SOIC packages. even got some lead free solder paste.Only help i think i need now is some review of my PCB. like i said, home etched, soic and 0805 and using solder paste. This not a professional product, i am only in high school. Just wondering if my design has any major faults.below are the board and schematic.the trace width varies quite a bit, i don't want traces to close to each other or to thin because i am etching this. Thick traces have better chance of working out.

author: Buriedcode
author_rank: Super Contributor
timestamp: May 23, 2017, 11:16:58 pm
content: Not bad, especially for someone in high school0805 and SOIC are definitely solderable by hand, even without solder paste. The key is flux. Preferably gel flux - stuff tahts specifically for electronics, as there's various corrosive types for plumbing/welding that will do more harm than good.Circuit:Are you sure the Attiny has internal pullups on the switch inputs? (it might, I just don't know). Does the ahll sensor require a pull-up/down resistor on its output? What happens if you;re software makes that an input? will it fry the hall sensor?Schematic: I see you have some nets/wires criss-crossing a lot. Also, the many bends in a net can be confusing. Remember, you don't have to shrink it down, you have plenty of space and can separate areas into groups. Say, LED's with their respective resistors bottom right, switches top right, hall sensor top left etc.. It's readable! But perhaps could be neater. JP1 - JP10 I assume are just for off-board wires. Although space is limited and it won't show up on a DIY PCB anyway - changing those names to something meaningful might help you later on when you're actually wiring it up.As for the PCB, a few comments.- some traces are awfully close together. This might not matter that much for professional made boards with 4mil spacing, but for DIY? You want the largest gap as well as the largest trace width you can fit on the board.Whether you're using the 'press'n'peel' (toner transfer) method, or UV exposure method, don't make life more difficult by having very small traces/gaps.- Where the resistors connect to the micro, although they can just be straight traces off the pins, I find it can be neater to only use 45 degree angles- The foot print for the hall sensor has lads that are very close together. You could change the foot print to use round pads, of a smaller diameter, but if they require say 0.6mm holes, reducing the diameter leaves less copper around the edge - so makes it easier to tear off the pads whilst drilling. I would use SMT pads for that, and if your idea allows, solder the hall sensor on the component side.- I'm sure you're aware that blue is the bottom layer, viewed from the top.. thus the mirror text. Nothing wrong with this at all, but if most of the components are on the 'component side' I tend to make this top (red) and mirror everything that goes on the bottom. This way it looks on screen how it would look in reality. But it also means if you're using press'n'peel/toner transfers you'll have to mirror the image again before printing. Gets very confusing! As it is, you could print that off and as the bottom is already mirrored... it'll be the right way around for toner transfer.- You have polygons/islands that are not connected to anything and are very close the tactile switch connections. Generally, one would make a polygon the GND (or power, but often ground) and draw over the whole design, letting the CAD software sort out clearance. Also, you can set this clearance, for my DIY boards 16mil clearance was the closest I ever needed.- I can't see any *major* faults, but some niggles, like traces not coming directly form the centre of SMD pads, and as mentioned so very tight clearances. Run a DRC (design rule check) and set some clearances to say 10mil. It will highlight where it fails these checks.If you're using eagle ver 5.11.0, or 7.5.0 and want someone to tidy it up (along with steps of *how* they did it) attach your eagle files and I'll give it a bash. I don't have the latest eagle version, and I don't really want to install a 4th version.If that is your first effort, 8/10 sir.

author: Yansi
author_rank: Super Contributor
timestamp: May 25, 2017, 01:09:35 pm
content: QuoteCompletely missing decoupling capacitors noone?