What are the top "traps for young players" in basic PCB design?  - Page 1
Forum section: electronics / beginners

author: futurebird
author_rank: Newbie
timestamp: April 28, 2016, 07:05:56 pm
content: What are the top "traps for young players" in basic PCB design? I'm learning Eagle and I'd love to know what to avoid. Is there an intro level book on this topic?To give you an idea of my level: I'm working my way through Art of Electronics by doing the exercises. I'm on the second chapter. I'm a mathematician (college prof) by training, but I've been thinking about a career shift. Anyway, my plan for now is to study the book and build lots of projects. I might take a course in the fall if this continues to go well. I've made a few simple PCBs and they work, I used "fritzing" but I'm already finding that software a bit limiting.There are a lot of good resources to get stared with PCB design. And plenty of advanced stuff that is over my head (for now.) A list of common errors would be really helpful. Or reading/watching a critique of a beginner's design.I hope this isn't too general!Also, hello! I've gained so much from this forum and Dave's videos, but this question has been nagging me so I finally had to stop lurking.

author: rstofer
author_rank: Super Contributor
timestamp: April 28, 2016, 07:52:41 pm
content: I would suggest getting a sufficiently complex PCB (maybe an FPGA development board or perhaps a PC motherboard) and looking at it for things that scream "that's odd".For example, heading toward memory chips you will see S bends in the traces to achieve equal distance or perhaps even certain delays between signals. I know, 1.2 nS per foot but we're dealing with 10s of picoseconds.Trace cross-sectional area versus current.Trace clearance versus voltage (applies to higher voltages, like mains)Capacitance and inductance are always a problem, when they are unwanted.Pad sizing - small pads are harder to solder, very large pads work like heatsinks.Speaking of heat sinks, look for via holes between heatsinks on the top and bottom layers.Inner layers for power and ground - typical for 4 layer boards and the only way they make them at ExpressPCB. Signals have to be placed on the top and bottom layers.These are the most trivial of considerations. I'm not a great PCB designer but my boards work so I'm happy. Most of my projects work in the low MHz range, nothing approaching the GHz range.I have never gotten up to speed on Eagle. The learning curve is just a lot steeper than I am willing to climb. I use ExpressPCB (and their free software) for all of my projects.

author: tautech
author_rank: Super Contributor
timestamp: April 28, 2016, 08:01:30 pm
content: Welcome to the forum.See recent thread:https://www.eevblog.com/forum/projects/how-difficult-it-is-for-hobbyist-to-work-with-smd-packages/

author: KL27x
author_rank: Super Contributor
timestamp: April 28, 2016, 11:08:52 pm
content: My own mistakes1. Using a proprietary free software because of its simplicity. I would recommend just don't do it.2. Designing a simple board without a schematic, using just the pads. Again, I would recommend just don't do it. Make a schematic.3. Check your solder paste layer. Some things you want pasted, some you don't.4. For non-leaded parts, extending the pads beyond the edges of the chip will reduce your time spent trouble-shooting, even if you use paste/reflow. Visual inspection will reveal bead or no bead. That's a pretty good start.If you reveal what software you use, you might get a heck of a lot more specific, practical tips.

author: tggzzz
author_rank: Super Contributor
timestamp: April 28, 2016, 11:27:30 pm
content: Quote from: KL27x on April 28, 2016, 11:08:52 pmHe's interested in understanding what makes PCBs work and fail, not which button to push in one specific package. The information he's after will be current and relevant long after any specific package has crumbled into bitrot.

author: tec5c
author_rank: Frequent Contributor
timestamp: April 29, 2016, 12:43:41 am
content: Quote from: tggzzz on April 28, 2016, 11:27:30 pmAlso, he did say what software he had been using - 'Fritzing'.Futurebird, as you said you are finding Fritzing to be a bit limiting. Have you tried Eagle? You can download it for free from here:http://www.cadsoftusa.com/download-eagle/I refer you to a document written by Dave that tends to go unnoticed. It's a decent starting point for someone getting into PCB design.http://alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

author: MarvinTheMartian
author_rank: Frequent Contributor
timestamp: April 29, 2016, 12:56:38 am
content: QuoteI would second that!I found this document long before I knew of Dave's videos and the forum.

author: alexanderbrevig
author_rank: Frequent Contributor
timestamp: April 29, 2016, 01:01:23 am
content: Thank you tec5c! I've never seen that resource linked. Just read it and I wish I had found it a year agoMy list of traps would be:Not understanding DRC error messages correctlyIf DRC complains, find a way to fix itNot checking the gerber files for mistakesTriple check solder mask layer and solder paste layer if you make a stencilMake sure you make your footprint from the correct drawing in the datasheet (some are from the bottom up)When you discover you've made an error. Make sure you don't repeat it!

author: Apollyon25_
author_rank: Regular Contributor
timestamp: April 29, 2016, 02:28:04 am
content: Practice, practice, and practice, and I'd second the 'don't repeat a mistake' message.My first ever board (using CAD software) - I finished it, was asked, did you run a DRC? Yup. Cool, go make it.Etched, drilled, populated and powered it up. Nothing worked. You sure you ran a DRC? Yup.Show me. (Early version of Altium/Protel/Autotrax) click tools, click DRC check. <whirring> "DRC check complete" dialog box with an "Ok" button.Did you look at the log file?What log file?(Cheers TG!)There is nothing like practice. So after this embarrassing incident I spent may months re-drawing/entering/designing a plethora of old Electronics Australia, Silicon Chip, Elektor projects. Then I sent them all of to get made and built them. And I got heaps of cool gadgets/tools/equipment out of it.Now, when I run DRC's I account for every message and either fix it, or note it's reason as part of the review stage.I also get others to review my designs - this gives a fresh set of eyes looking over it, which sometimes picks up things I've missed, or utterly forgotten. You also get the benefit of their experience so you avoid THEIR mistakes too.

author: Kjelt
author_rank: Super Contributor
timestamp: April 29, 2016, 09:55:10 am
content: Dave (creator of the forum) wrote a guide for pcb design:http://www.alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdfto add two off my own mistakes:- never use wires but use nets(unless you have no other option for instance wiring two groundplanes together you can use wires just name them the same as the groundplane)- if your pcb needs an enclosure (or might need it) first buy the enclosure and use its cad drawings for the mounting holes on the pcb.tips:You need to learn where goes what, first pcbs you probably will stick some components somewhere and start to find out an hour later that was not the best positionNever use the auto router untill you are an expert and then you probably will not use it anyway.With components you have not used before and are unsure about the footprint, print the pcb out in 100% scale put the component on top under a microscope and double check if it fits.

author: futurebird
author_rank: Newbie
timestamp: April 29, 2016, 10:13:26 am
content: Thanks for the links and tips from your experiences. As for software, I was using fritzing, but now I'm getting started with Eagle. I may look into some of the other software mentioned since fritzing, though easy, is very limiting.PS. I'm "she" not "he"

author: Kjelt
author_rank: Super Contributor
timestamp: April 29, 2016, 10:18:10 am
content: If you want to make it your career I would suggest looking at the pro pcb packages, like Altium.I believe they now also have some free web version never looked into it myself but this forum should have many posts about it.But I am not sure what you mean with careershift, if that means you would like to make pcb's as a living or as teacher to students?I use eagle myself since it is cheap and does what I need which is not much, but to be honest it has many limitations and is not evolving as it should have.If you have to start over from scratch I would also open a topic asking which pcb software the users here would advice for the exact carreerswitch you have in mind.

author: Alex Trofimov
author_rank: Contributor
timestamp: April 29, 2016, 11:01:18 am
content: Use only the footprints that you (or your team) did yourself and tripple check all the measurements)

author: Apollyon25_
author_rank: Regular Contributor
timestamp: May 01, 2016, 09:03:47 pm
content: I agree regarding using a professional version of software - If you are considering a career shift, it would be beneficial to learn at least one of the standard packages. PADS, Cadence/Allegro or Altium are the most prevalent (certainly here).I haven't used Circuit Maker (I have full licenced versions of Altium both professionally and personally) however it from all appearances is very similar to Altium Designer so that might be a better first choice than some others.Though most of the big packages will have entry-level/maker-space versions.If you like, feel free to send me any designs you have done to date, and I'll be more than happy to review and suggest improvements.A couple of pearls of wisdom regarding layout which have stood me in good stead over the years are:Current flows in loops, and always follow the path of least inductance/impedance.When you obey these, for RF, for high current signals, for fast digital edges, for high impedance analog inputs, and for noisy switch-mode supplies, your designs will be considerably more robust and quieter for EMI/EMC.Its really just about understanding the signals and the compromises you choose to make.

author: Apollyon25_
author_rank: Regular Contributor
timestamp: May 01, 2016, 09:31:49 pm
content: Quote from: blueskull on April 29, 2016, 10:16:58 amI'm going to largely disagree - especially in the context of "this is for a beginner"a) Soldermask expansion is simply a ratio of soldermask aperture to pad dimensions. Do you mean to tell me you don't have soldermask on your PCBs with BGAs? I don't think so.b) Relief connects serve a particular purpose, and whilst your statement under standard reflow techniques in commercial CMs may prove true, for hand soldering relief connects are preferred to alleviate micro-cracks, and to simply make hand soldering easier.c) Again acute and R/A traces have their uses, but best practice is to not use them. If you have to, it should be a conscious decisions with an understanding of the signals involved and the impacts of doing so. Any kinks, cause increased current density in the corners, increasing localised dissipation and radiated fields. Typically this isnt an issue, however it is very application dependent.I have mixed views on digital terminations and these tend to be fluid and specific with the design in question.d) Trace thickness depends again on the CM and board fabricator. There is often no need to have ridiculously small traces, and for a beginner, which is whom we are doing this for, the likelyhood of them doing BGA design is very remote. If you go beyond the minimums recommended by the fabricator, you need to appreciate that the reliability and yield may go down and the subsequent cost to cover that yield will go up. "Can they?" is a different question to "Will they?", but the issue here is "Should you?"e) IPC rules for current traces - again the adoption of IPC-anything is a matter of choice. I know for a fact that not all power electronics designs ignore IPC recommendations. Having designed a fair amount of it previously. But as a guideline for a beginner, they provide an easy first step. Deviation is a design decision balanced against other tradeoffs.f )Package sizes are contentious. Sure they increase available board real estate, but at the expense of ease of maintenance. Unless I absolutely have to, I will always pick leaded parts (QFP etc) over QFN/BGA. Purely from a re-work point of view. This all depends on the rework tools at your disposal of course. I can rework BGAs with a preheater and a hot air station - do I like doing it? Hell no. Getting 300 odd pins soldered reliably is a PITA! For a hobbyist? Pick whatever packages you are comfortable working with. I used to hate 0402s, now I dont mind them, I'll even tolerate 0201s. Would I expect a beginner to rework these? Absolutely not. 1206/0805s sure, 0603's debatable.

author: Apollyon25_
author_rank: Regular Contributor
timestamp: May 02, 2016, 12:29:37 am
content: So a beginner will note from this that there are differing viewpoints depending on the tools available, experience/familiarity level etc. What works for hot air, doesn't necessarily work with a soldering iron. Designing for mass production with a CM is also somewhat different too.Which is to say, following best practices and IPC recommendations and all this stuff only gets you so far, and each decision needs to be weighed up against the design goals.Also, I have seen the effects of micro-cracks on MLCCs at <5V. This is still a problem in the industry.However a beginner is probably not going to encounter this.

author: bson
author_rank: Unknown
timestamp: May 02, 2016, 01:59:29 am
content: If you use a part for the first time and create/adopt a footprint for it, print the footprint on paper at 100% and place the part on it, on the paper printout, to make sure it matches. Not talking magnification variations in the print here; you'd beamazedhow ridiculously easy it is to use the wrong footprint for MSOP/SSOP/TSSOP parts. As in, completely off no chance in hell of getting it soldered on there not even freaking close. They come in a stunning variation of widths and it's super easy to make a mistake when just looking at the package drawings on the datasheet. You'd think not. But trust me... print and verify. (And this doesn't even include complete brain farts like using an SSOP footprint for an op amp that only comes in DIP or SOIC, because... well... who the hell knows why!)

author: Jeroen3
author_rank: Super Contributor
timestamp: May 02, 2016, 08:34:26 am
content: Don't do this with qfp's. Can you spot it?

author: tautech
author_rank: Super Contributor
timestamp: May 02, 2016, 08:42:42 am
content: Quote from: Jeroen3 on May 02, 2016, 08:34:26 amPads 4&5, 7&8

author: stmdude
author_rank: Frequent Contributor
timestamp: May 02, 2016, 09:57:23 am
content: 1. Footprints (like everyone else has said). Check, and double check2. Trace widths. Bigger is almost always better (until you reach impedence controlled tracks)3. Ground-return. If you have big beefy power-tracks doesn't matter if your ground-return is small and wimpy.

author: futurebird
author_rank: Newbie
timestamp: May 02, 2016, 04:38:09 pm
content: Quote from: bson on May 02, 2016, 01:59:29 amThis is really helpful. I need to add the "paper fit" step to my process for home etching. I made a one sided board last night mis-judged which side a part would end up on. Had to re-do the etch. I'm going to try to take the advice given by one of you not to make the same mistake twice.

author: jolshefsky
author_rank: Regular Contributor
timestamp: May 02, 2016, 07:19:24 pm
content: Here's somehints from Sparkfunon their designs (from 2008). I could swear they posted a checklist at one point (e.g. things to check prior to making a board) but I couldn't find it but I had made my own based on it:Confirm ERC on schematic.Print schematic and review.Silkscreen board name, version, date, creator, company.Silkscreen version information from CVS.Check size of PCB edges against specification.Check for unconnected nets.Confirm DRC on board.Check Gerbers in local software.Print board at 100% size.I think a general rule that covers a lot of what has been suggested is, "don't rely on someone else's work until you understand how to do it yourself." Footprints are a big example: in both Eagle and now KiCAD I started out trying to use their footprints, but after having problems I now always make my own for each part based on the diagram in the datasheet and the suggested landing pattern.

author: Apollyon25_
author_rank: Regular Contributor
timestamp: May 02, 2016, 08:45:11 pm
content: On the topic of library parts, I'm not sure what capabilities other packages have, but Altium allows you to put the designator and comment (usually value/PN) as special strings in the component footprint, on whatever layer you like pre-arranged and pre-positioned.This means for densely populated PCB's you simply can turn off the overlay layer (if you want) and have all the designator and values all set up on layers ready for printing/viewing. Saves you repositioning every piece of text on the board to be visible.Print this layer really big, and with the BoM for qtys, hand placing is loads easier.The other thing I do is create on a mech layer the physical body outline and a clearance area outline (IPC - N density typically), along with a centre of body crosshair and a pin one mark.This lets me place components tightly together quickly, knowing I'm not going to have placement (machine) issues.If I need to then nudge other components and test points closer I can see on the mech layer if there is any clearance issues from component bodies.

author: basinstreetdesign
author_rank: Frequent Contributor
timestamp: May 04, 2016, 01:58:25 am
content: I must add one more bugaboo that seems to crop up any time I'm not watching and that is making sure that the footprint and pinout of three-terminal devices match between your schematic program and your PCB layout package. This has happened I dont know how many times all during my career. Take a 2n3904 transistor which has three leads and made by many manufacturers who do not agree how the pin numbers should be assigned. If you use a 2n3904 from the schematic library and it gets linked to a TO-92 NPN transistor footprint from the layout library then those three leads have six different ways of being connected. Chances are yours will be the wrong one. If your design uses 24 of them and you are making 6 boards to start then you are in for a lot of re-work.This kind of thing applies to diodes as well since the libraries may use pin numbers 1 and 2 or K and A. As well the pin assignment for diodes can be screwed up by the same above issue.Interestingly, as soon as the device in question gets four pins the problem seems to go away.To guard against this kind of thing, make sure your PCB checklist (has anybody yet mentioned just how good having a checklist can be?) includes checking 2, 3 terminal devices for footprint against the datasheet by the actual manufacturer you will be buying your stuff from.Tim

author: jolshefsky
author_rank: Regular Contributor
timestamp: May 05, 2016, 03:01:53 pm
content: Quote from: basinstreetdesign on May 04, 2016, 01:58:25 amGood one. I should add that to my list.My own libraries in KiCAD tend to lean on the "labeled" pins approach (e.g. BCE rather than 123). I think it's slightly more error resistant since if you take an NPN with pins named BCE and use a footprint with 123, none of the pins will be connected and it'll immediately be weird when doing layout. The trouble is the footprint count expands proportionally, what with the three order combinations and adding things like FETs and voltage regulators, all the sudden there's a lot of three-legged parts out there.What would be needed, I think, is an intermediate step between schematic-part and layout-footprint where one maps the functional pins of a schematic to the functional pins in a specific device which THEN maps to the physical pins of a package. I should, then have just one TO-92 package in the library which could be related to any number of devices.One thing I think was a win was to use C/NO/NC on all the switches in the libraries and footprints. So if I have a normally-open pushbutton in a schematic, it's got a common (C) and normally-open (NO) pin and I can use practically any switch as a footprint. Multiple poles get annotated starting at 1 (C1, NO1, C2, NO2, etc.)

author: Cerebus
author_rank: Super Contributor
timestamp: May 06, 2016, 01:32:14 am
content: If you have enough layers, a ground plane will take away an enormous amount of pain in anything fast, sensitive or noisy. If you don't have enough layers use polygon pours for ground wherever you can.

author: kendalll
author_rank: Contributor
timestamp: May 07, 2016, 09:32:08 pm
content: Home etching a pcb seems like a waste of time and effort when there's options that are pretty affordable and reasonably good quality.https://oshpark.com/pricingI mean unless the process of doing it at home is really fun for you...