PCB Design Critique - Universal RFID Card - Page 1
Forum section: electronics / projects

author: bentx0rx0
author_rank: Contributor
timestamp: March 21, 2014, 05:20:56 pm
content: Hello! I thought I'd ask for your opinion on a schematic and board I've laid out using Eagle. It's not my first board, but I thought you guys might be able to provide some suggestions for better boards in the future.It's designed to act as a multi output 125kHz RFID card, for the RFID readers that only send a key(cheap chinese ones). It features an atmega328, a boost regulator for lithium ion and single AA power cells, and that's about it. I left the 328 as through hole so people could pull the chip out and reprogram it instead of using the ICSP header.Things I know:1) I haven't added silk labels yet. I will have plenty.2) Something about the power supply on the bottom layer bothers me.I'm still a bit new to Eagle, I've been using Kicad extensively. Let me know what you guys think!Schematic:https://www.dropbox.com/s/cpe1eqaj941xt96/mainthru.schBoard:https://www.dropbox.com/sh/6ro3aigza6g315r/I3TK8-LY_z/mainthru.brdSchematic Image:Board Image:

author: free_electron
author_rank: Super Contributor
timestamp: March 21, 2014, 06:24:59 pm
content: post pdfs or screenshots. no way i am installing eagle...

author: 8086
author_rank: Super Contributor
timestamp: March 21, 2014, 06:27:17 pm
content: Quote from: free_electron on March 21, 2014, 06:24:59 pmSeconded.

author: bentx0rx0
author_rank: Contributor
timestamp: March 21, 2014, 06:34:42 pm
content: Done. Note that there's a ground polygon I didn't fill to make it easier to see.

author: daedalus
author_rank: Regular Contributor
timestamp: March 22, 2014, 12:55:39 am
content: as you have turned off your ground pour polygon you might have covered some of this already, but here are the changes I would make:0) where is the decoupling cap for U1?1) try to have the crystal and caps on a ground pour, without other traces running through it.1)I cant tell where everything is, but your layout for lm2621mm needs work. Youshould aim to keep the current loop as closely routed as possible. Ideally the entire subcircuit should have a ground pour round it. Try looking at a reference design for lm2621mm, such as LM2621EVAL and note how tight the caps/inductor/diode are to the ic.2)You have smt parts, but a through-hole micro, if you swapped to an smt micro you could probably reduce the board space required, freeing up some space. Personally as soon as I have smt parts, I go all smt, so I would swap clock and header to smt, but the last ones just a personal preference.3)You have double side loading on this board, but you probably have space to do everything single side load. This will make assembly easier.4) do you really need a reset button for micro? its only ever gonna get used during dev, you could just power cycle5) could you explain what jp2 + rectifier is trying to achieve?6) some mechanical fixing points, like screw holes might be usefulEdit: spotted a cap was missing

author: free_electron
author_rank: Super Contributor
timestamp: March 22, 2014, 04:31:35 am
content: Where is your inductor ? (Rfid) that is a very sensitive line !

author: bentx0rx0
author_rank: Contributor
timestamp: March 22, 2014, 06:07:53 am
content: There's the inductor in the bottom left for the power supply, but I must have forgotten the one for the RFID circuit.

author: daedalus
author_rank: Regular Contributor
timestamp: March 23, 2014, 12:27:10 am
content: Ben, one thing I didn't make clear in my last post, please don't take the long list of suggestions as anything but constructive criticism, when I was starting out some of my first boards would have had a much longer list, its all part of the learning processwith regards to the RF side, this isn't my area so was avoiding commenting, however what you are building seems quite similar to this device.http://www.proxclone.com/spoofer.html.Analysing the analog side of that is not trivial, it might be best to start off by using a tested known good design, then make your changes incrementally.

author: bentx0rx0
author_rank: Contributor
timestamp: March 23, 2014, 12:34:11 am
content: Don't worry, I'm not offended by your comments. I was asking for improvements. The regulator layout was very sloppy of me, It's a lot harder for me to see the back side of the board when I've got polygons as a ground pour, but there's no excuse. The design is almost an exact copy of a very similar Instructables project.Is that inductor an inductor, or the inductance of a certain number of wire turns? I see the same thing in the Qi Power Standard, Design B1. I guess I assumed it was the coil inductance and not a needed component. Is this accurate, or is it a physical part?RF is very new and interesting to me, so I thought I'd do a few more RF related projects. I've got Chris Bowick's book RF Circuit Design, and I'm working my way through that. Thanks for the advice daedalus and everyone

author: daedalus
author_rank: Regular Contributor
timestamp: March 23, 2014, 12:51:20 am
content: i must admit RF isn't really my thing, but from my understanding the inductor in the design is actually your transmit/receive coil, which should be around 1.6mH, and connected close to C1. All of this part of the circuit is noise sensitive, and should be kept away from the switching dc-dc. with regards to lm2621, there is a tool on TIs website that will recommend optimal caps/diode/inductor, this can be useful in saving time on one-off designs.http://uk.mouser.com/images/texasinstruments/lrg/lm2621eval.jpgshows a good layout for the chip, its mostly single sided with 2 vias.the thing to note in this design is the tight loop between inductor diode, caps and IC. keeping this area small reduces EMI issues.

author: FreddyVictor
author_rank: Regular Contributor
timestamp: March 23, 2014, 08:59:46 am
content: Quote from: bentx0rx0 on March 23, 2014, 12:34:11 ama tip to help with this:to clear (but not delete) the polygon fill, use the 'ripup' tool on the polygon line edge