Surface Mount PCB Critique - Page 1
Forum section: electronics / beginners

author: RJDog
author_rank: Contributor
timestamp: February 14, 2017, 02:39:13 pm
content: So as I've mentioned recently, I'm pretty confident in my design and assembly ability for through-hole boards and components, but this is my first foray into surface mount components, so I am hoping to garner some feedback from you guys along the lines of "yeah, that will work for you" or "you shouldn't do X because Y" for the main surface mount components.The three chips shown are SOIC-14, and I've modified the footprint to make the pads 1mm longer (away from the chip, of course) to aid in prototype hand assembly. As a design principle, I tried to make all of the vias directly in front of the pad they're attached to; not sure if that is actually a good design idea or not, but I seemed to be able to make it work for this simple layout. Incidentally, I've never had to use so many vias, but I suppose that's normal with SMT?U1 is a 74HCT125, U2 is a 74LVC125, IC1 is an Atmel AtTiny441. Also, as a side(ish) note, I want/need to feed U1 with a 3.3V supply and U2 with a 5V supply, as I am primarily using them for logic level translation, but the KiCAD schematic editor doesn't seem to be letting me supply both chips with different supply lines... it has pin 14 (Vcc) of both chips bonded somehow? Consequently, I had to manually edit the exported netlist to make it work the way I want in pcbnew. Anyone else have this problem, or am I missing something?

author: alexanderbrevig
author_rank: Frequent Contributor
timestamp: February 14, 2017, 02:54:33 pm
content: Some quick comments from my phone.Your layout seems reasonable, I would try to spread tracks instead of grouping them, you have one or more 90degree angles. This probably won't matter much these days though, still good to get in the habit of avoiding them (and above of course). Lastly if your fab house sports less clearance and three are low speed signals you could fit a trace between each pin of those ICsfrom my phoneEDIT: just noticed the lack of decoupling, you should look into that

author: wraper
author_rank: Unknown
timestamp: February 14, 2017, 03:09:42 pm
content: I don't like quartz oscillator layout. Also what the the point in using through hole passive components?I don't see any decoupling capacitors as well.

author: RJDog
author_rank: Contributor
timestamp: February 14, 2017, 03:24:42 pm
content: Quote from: alexanderbrevig on February 14, 2017, 02:54:33 pmI've never had a problem with 90 degree angles before... I was not aware that this was to be avoided?The fab does support 6mil (at least, without costing exponentially more) clearance, but I think I would like to avoid putting traces between pads... or am I silly for thinking so?Yeah, decoupling capacitors... we're talking about the nice guys to cut out transients near the Vcc supply of each IC? I suppose I should put some of those in there, I totally forgot. I assume the placement is the same as you would with through-hole IC's -- nearest the Vcc supply pin to nearest ground fill?Quote from: wraper on February 14, 2017, 03:09:42 pmI'm interested in your thoughts on the oscillator layout... this was actually one area I wasn't 100% on.Also, through-hole passives because I've got about a billion of them lying around, and it's a prototype...

author: JPortici
author_rank: Super Contributor
timestamp: February 14, 2017, 03:38:50 pm
content: usually there is a gnd pin next to the OSC pins, so that you have the shortest return path for the current on the oscillator... also to provide a guard ring (it's an high gain circuit) In the datasheet you should have a suggested layout for the oscillator

author: RJDog
author_rank: Contributor
timestamp: February 14, 2017, 04:12:30 pm
content: Quote from: JPortici on February 14, 2017, 03:38:50 pmNo GND pin next to the XTAL1/2 pins, nor recommended layout for the oscillator in the AtTiny441 data sheet..

author: hammy
author_rank: Unknown
timestamp: February 14, 2017, 04:19:41 pm
content: Quote from: RJDog on February 14, 2017, 03:24:42 pmI wouldn't route the reset-line near and around the xtal (no gnd?) like this. Maybe it is possible to route it on the other side from pin4, underneath IC1 down?

author: wraper
author_rank: Unknown
timestamp: February 14, 2017, 05:35:58 pm
content: Quote from: RJDog on February 14, 2017, 03:24:42 pmYou run traces very close to the crystal traces under the capacitors. You don't want any signals messing up with your oscillator. Best case you have only GND around your oscillator.QuoteWithout them and depending on how close any other capacitors are on the power rail, your circuit may be unstable or not work at all.

author: tautech
author_rank: Super Contributor
timestamp: February 14, 2017, 08:01:17 pm
content: For just a few $ you can get 0805 passive kits and their use will change the layout somewhat for the better. On a SS PCB you might want to drop in the odd TH to provide routing paths but it shouldn't be necessary on a DS board.

author: RJDog
author_rank: Contributor
timestamp: February 14, 2017, 08:20:05 pm
content: Ok, revision 2, now with aversion to routing anything near the oscillator and related caps, added caps near the Vcc supply of the ICs, and some other rerouting as suggested...I really appreciate the suggestions re: the oscillator trace routing, and pointing out that I forgot the decoupling caps.

author: tautech
author_rank: Super Contributor
timestamp: February 14, 2017, 09:01:02 pm
content: Not that it might matter for this PCB but imagine trying to do rework on the IC next to the crystal.....one of the traps with SMD that you don't get with TH designs.TH components are much better where you have shifted them to.

author: james_s
author_rank: Super Contributor
timestamp: February 14, 2017, 09:22:14 pm
content: Yeah 90 degree bends are best avoided, generally they will work, but that and oddball angles are a sure way to identify a board designed by an amateur. Look at PCBs in commercial products and they will usually have 0, 45 and 90 degree trace angles only, and 45-45 bends rather than 90 degree bends. It's not a huge deal, it mostly looks nicer and if you etch boards at home it increases yields.I try to avoid through-hole parts as much as possible, it's much faster to assemble a purely SMT board, but I usually use a hotplate to reflow solder. If you're installing individual components it makes less difference but I still hate forming the leads and snipping off the remnants.

author: FrankT
author_rank: Regular Contributor
timestamp: February 15, 2017, 07:59:21 pm
content: Quote from: james_s on February 14, 2017, 09:22:14 pmIs 90 degrees an issue?I was reading an article (can't find it now - circuitstudio documentation, or blog) where the author said it isn't an issue these days. 90 degrees was a problem with the old ways of etching PCBs where the inside corners would over etch, reducing the width of the tracks.

author: tautech
author_rank: Super Contributor
timestamp: February 15, 2017, 08:12:20 pm
content: Quote from: FrankT on February 15, 2017, 07:59:21 pmNo more than a trace running through a TH pad with a default annular ring size. (too small)At some point you will need to branch off from a net and invariably it will be @ 90 degrees.Never had a problem with my home etching with traces coming off at 90 and never felt the need to add fillets to prevent undercutting. Push the limits to a silly 6 mil or similar, then you are inviting all manner of unforeseen problems.It's a myth.

author: mrpackethead
author_rank: Super Contributor
timestamp: February 15, 2017, 09:08:00 pm
content: why dn't you remove your TH passives?

author: james_s
author_rank: Super Contributor
timestamp: February 15, 2017, 09:25:58 pm
content: Quote from: FrankT on February 15, 2017, 07:59:21 pmFor the most part, no, not anymore, though if you etch your own boards at home, which I do occasionally using toner transfer, 90 degree bends are more prone to bad etching. Mostly it's just a visual thing, a 45-45 bend looks more pleasing and professional. Yeah, I know, who cares what a PCB looks like right? Well I'm not going to deny having some minor OCD tendencies but a good PCB layout is a work of art. It's one of those things like trimming the outer sheath of Romex back to within a half inch of the box entry as mandated by (US) electrical code, it doesn't *really* matter in most cases but you can tell at a glance that the job was done by an amateur if that hasn't been done.

author: Vtile
author_rank: Super Contributor
timestamp: February 15, 2017, 09:53:26 pm
content: There is also some theoretical significance to avoid sharp corners, but I'm not sure if PCB traces ever carry such a currents it would make any difference.

author: tautech
author_rank: Super Contributor
timestamp: February 15, 2017, 10:02:36 pm
content: Quote from: james_s on February 15, 2017, 09:25:58 pmTrue, but only if you are not using a bubbler etching bath and with TT porosity in the toner of far more problematic, moreso with fine traces.

author: alexanderbrevig
author_rank: Frequent Contributor
timestamp: February 16, 2017, 12:04:04 am
content: Hi again RJDog!90 degree angles can cause what is called an acid trap, worst case the acid will eat through your trace. Not often an issue, but not a myth either.Another thing to consider, for RF for instance, is that the impedance actually changes quite a lot (thank you Pythagoras). You'll often see round traces when RF is involved. Still though, it's considered a best practice by most.When you need a T from from say a power trace, then add fillets. Looks better (wow, someone actually thought here!) so if only for that - do itYou're not wrong for thinking traces between pads is bad, it's much better to avoid. If you're interested in it, read up on crosstalk and series terminationCorrect about the decoupling. Another best practice here is to route the power to the cap, then to the pin. Not sure it has all that much effect, but it's what I do because everyone else does it that way.With high speeds, the oscillator should be routed such that each trace is as short and as equal as possible. The RST lines should be far away any clocks.

author: KE5FX
author_rank: Super Contributor
timestamp: February 16, 2017, 12:11:55 am
content: A few 90-degree junctions here and there aren't going to be a problem. PCB processes aremuchtoo tightly controlled these days for other reasons to allow the formation of acid traps. And trace geometry is a nonissue until you're working well into the GHz range.However, get into the habit of adding ground vias here and there whenever you find yourself creating large areas of copper. Those large copper islands are known by another name: "antennas."

author: james_s
author_rank: Super Contributor
timestamp: February 16, 2017, 01:06:36 am
content: I'm a believer in the saying that neatness counts. If you get in the habit of doing things "right" and producing professional looking projects there is overall a greater chance that they will work properly too. The more careful you are with the details, the less likely you are to make a mistake where it really does matter, and this sort of attention to detail costs nothing more than a bit of your time designing the layout. Neat tidy traces is just one of the finishing touches a craftsman puts on their work.

author: RJDog
author_rank: Contributor
timestamp: February 17, 2017, 11:09:42 pm
content: Thanks everyone for your comments; I definitely appreciate the explanation around the crystal trace routing (I have now moved all other traces totally away from the crystal, capacitors and pins on the AVR both top and bottom layers), and reason to avoid 90-degree traces (I have now put in fillets for traces that I still feel need to be 90 degrees, or otherwise avoided 90 degree angles where possible).