EEVblog #1129 - Creating a Nice Readable Schematic - Page 1
Forum section: electronics / general

author: EEVblog
author_rank: Unknown
timestamp: October 07, 2018, 05:45:53 am
content: How to turn a horrible unorganised schematic into a nice readable modular schematic with proper signal flow.Tips on industry expected layout techniques.Using the open source Haasoscope oscilloscope as an example.Please do NOT complain about the length of this video. I know. It is what it is.

author: Mr. Scram
author_rank: Super Contributor
timestamp: October 07, 2018, 05:50:15 am
content: The video is so long!I like it. In depth nuggets of knowledge that help me get from amateur hour to something slightly better is why I come to Eevblog.

author: eV1Te
author_rank: Regular Contributor
timestamp: October 07, 2018, 08:43:14 am
content: I found a mistake: 0.01 uF is 10 nF, not 100 nF as you converted it to in the video at about 45:00.It can also be written as 0u01, but not 0u1 nor 0n01 as you did.I won't judge you because I have confused myself with notations like in the past as well.Probably why you should stick to not using to many zeros after the decimal point in the first place. Hence your comments were spot on

author: Arznei
author_rank: Contributor
timestamp: October 07, 2018, 08:46:31 am
content: So much OCD triggering in this video. It's a real shame the Eagle import didn't quite work (regarding the grid), still enjoyed it though!I feel like the schematic could have really done with some multi-part symbols (I know you didn't want to mess around with them here), especially with the dual-OpAmps.What are your opinions on splitting up big components like the FPGA though? I think while splitting it up does seem reasonable (and I've seen it done quite a lot) you don't really gain anything by doing so. You either put all the parts near each other (often on a dedicated sheet) or you plaster them around your schematic wherever they are needed. The latter might tidy up your wires and spare you some net labels but at the expense of the FPGA now beeing all over the place, which I find pretty confusing if you want to check what the FPGA is doing in the schematic.What are the best practices here?

author: Icchan
author_rank: Regular Contributor
timestamp: October 07, 2018, 10:11:09 am
content: This video is really sorely needed one. From now on, if I see horrible schematics I can refer to this one and be done with it.It would be really nice if you released the tidied schematic as a PDFAND as a source file. Even if it's Altium format, it would be a good gesture towards OSHW community regardless.I believe you have a GitHub account?Thanks for the video and length is warranted on this occasion. hmm... gave me an idea... maybe I could make a video that's a bit more structured and concise, with chapters and time stamps so thatpeople in a hurrycould learn the same ideas but with more scripted andoverly editedtmway?

author: EEVblog
author_rank: Unknown
timestamp: October 07, 2018, 10:38:43 am
content: Quote from: Icchan on October 07, 2018, 10:11:09 amSorry but no, it's too much work. The import screwed up a lot of things.The designed did an update a few days ago I didn't know about, I was using an old eagle import from last week.

author: Rutger
author_rank: Regular Contributor
timestamp: October 07, 2018, 10:49:14 am
content: The naming convention should be the number 1 tip. It was buried in the video at 1:12:00, and hard to find.I think David should make a 5 min version of this video and go over the 10 things on do's and don'ts.﻿

author: firehopper
author_rank: Frequent Contributor
timestamp: October 07, 2018, 11:45:42 am
content: or maybe just a top 10 things to do or not in a schematic?

author: wilfred
author_rank: Super Contributor
timestamp: October 07, 2018, 11:48:52 am
content: Quote from: Rutger on October 07, 2018, 10:49:14 amYep. 5min should mean it'll sneak in under 20. But I was thinking a condensed version would be really useful. More on what you should do only though.

author: EEVblog
author_rank: Unknown
timestamp: October 07, 2018, 02:24:29 pm
content: Quote from: firehopper on October 07, 2018, 11:45:42 amThose Top 10 Youtube channels sure do get a lot of views...

author: CJay
author_rank: Super Contributor
timestamp: October 07, 2018, 02:44:54 pm
content: Quote from: EEVblog on October 07, 2018, 02:24:29 pmIt's not a bad idea, top ten tips on how to create a readable schematic, top ten tips on how to lay out a board, top ten blah blah...Dunno how much work it'd be but it would be useful

author: www2
author_rank: Contributor
timestamp: October 07, 2018, 02:54:35 pm
content: What are the opinions about putting the value/part number inside the part than outside?Example:https://imgur.com/a/YfDt3Io

author: woox2k
author_rank: Regular Contributor
timestamp: October 07, 2018, 03:36:08 pm
content: Quote from: EEVblog on October 07, 2018, 02:24:29 pmI hate these things. Sure they give a lot of views since these are essentially just to trick our brain to feel like it learned something and release some chemicals that make us feel better. They are pretty much useless for learning something though. Our brains are not a simple databases capable of remembering random facts.That's why i cant understand why people insist you making shorter videos. I watched this one in one go and i'm sure that thanks to it being so long i can remember what you said there in the future too.

author: BrianHG
author_rank: Super Contributor
timestamp: October 07, 2018, 05:07:01 pm
content: Quote from: www2 on October 07, 2018, 02:54:35 pmWhen it is a large enough single IC component, where you wont be confused with pin labels, I SOMETIMES place the part number & designator in the middle. Otherwise, for caps and resistors, ICs with sub-components like simple gates, multi-op-amps, it's always outside, right side up, and organized.

author: Cerebus
author_rank: Super Contributor
timestamp: October 07, 2018, 05:12:45 pm
content: Quote from: www2 on October 07, 2018, 02:54:35 pmIn the example you give the lack of white space around the value text, and the 90˚ rotation of it both make it harder to read than the counter example. I'd say avoid that style except possibly for small 'illustration' style schematics where you have room for some white space inside the component boundaries.

author: jancumps
author_rank: Unknown
timestamp: October 07, 2018, 05:21:05 pm
content: Maybe the original designer imported parts of the schematics from somewhere else too? What other reason would there be to mix rectangle and zig-zag resistor symbols?

author: SL4P
author_rank: Super Contributor
timestamp: October 07, 2018, 05:30:21 pm
content: One tip I didn’t see, was - if possible -Place yourpower bussesfrom the ‘most positive’ at the top, to the ‘most negative’ at the bottom.You also *implied* layout with thesignal flowfrom left-to-right, but that should also go into the Top 10 important concepts.Very useful episode to repost! Thanks

author: Pentium100
author_rank: Frequent Contributor
timestamp: October 07, 2018, 05:57:44 pm
content: Quote from: woox2k on October 07, 2018, 03:36:08 pmIf a video is too long, people may not have enough time to watch it or they might get bored.Anyway, when I draw a circuit diagram in Multisim, I usually make it pretty (unless it's something I won't even save), but when I have to do it in Eagle (if I want to order a PCB), then I'm happy it's readable enough so that I can find how everything goes togther as adjusting everything is really annoying. and, in the end, probably nobody else is going to see the schematic anyway.I always connect everything, using buses if there are a lot of digital signals. I hate it when I have to look around where "DATA_74" goes in a service manual. I can follow a line though. I'd rather read something liek this (attached, a circuit diagram of a tape deck) over the disconnected parts. Even though the tape deck has separate boards and modules, the circuit has them all connected together.Then again, I am not a professional.

author: chris_leyson
author_rank: Super Contributor
timestamp: October 07, 2018, 07:19:23 pm
content: Nice video Dave thanks, it will teach newcomers without much schematic drawing experience one hell of lot. Not only did you show good industry practice but you also explained why it's done that wayThings that perform certain functions have their own blocks and very easy to follow the signal path, nice job very well done.On a few occasions I've seen schematics drawn from right to left, several of those were because the design engineer was left handed and on one occasion I had a right to left schematic pop up at an interview, I was a bit perplexed trying to follow the signal path and I didn't get the job, no worries though. MInd you on the other hand, no pun intended, I worked with another left handed engineer who drew his schematics from left to right. My late younger brother was left handed and watching him "push" a pen across the page and not smudge think ink was something else.Do left handed engineers have a preference for drawing from right to left ?

author: akowalczyk
author_rank: Contributor
timestamp: October 07, 2018, 07:32:50 pm
content: Definitely using this as a teaching tool for new interns/co-ops. Can we have an equivalent for PCBs where you start from a bad one and make it good as well?It's a better course in schematics than four years of engineering school in the course of an hour and a half. This is really the type of learning that happens when your boss hands you back your schematic covered in red ink.I mostly avoid pins on the top and bottom, just looks cleaner in general, and lots of named nets rather than long nets connecting blocks. Tends to help when you run out of page space and have to add another, you just switch those net names to off page references.Also would've been nice to mention multi-symbol parts and separating out hundred-odd-pin chips/connectors into a handful of symbols with logical grouping (i.e. by banks, functions, power etc)

author: SL4P
author_rank: Super Contributor
timestamp: October 07, 2018, 07:42:18 pm
content: Sounds like some ideas for a full, multi chapter tutorial...Perhaps open-source, with fees for republishing...?

author: Cerebus
author_rank: Super Contributor
timestamp: October 07, 2018, 08:17:33 pm
content: I haven't had time to watch the video yet, so my apologies if I'm about to suggest something that Dave tackles at length in it.One rule I'd advocate is to draw typical sub-circuits in standard form.What I'm talking about is something like a differential pair of transistors. If you draw then in the classic form, shown here as A, then the sub-circuit's function is immediately obvious. If you draw it in non-standard form (B here is one possibility) it takes some thinking before you 'see' a differential pair.Another examples might be class B complementary output stages. I'm sure that many of you can chip in with design elements that you think should get this kind of treatment.

author: nctnico
author_rank: Super Contributor
timestamp: October 07, 2018, 08:24:14 pm
content: And don't draw swastikas...

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: October 07, 2018, 08:35:00 pm
content: The thing I hate most is when people just plop down all the symbols, with net names but no interconnect wires at all & call it a schematic.That, and not providing a PDF version in addition to the format of whatever tool they use

author: Mr. Scram
author_rank: Super Contributor
timestamp: October 07, 2018, 08:35:29 pm
content: Quote from: nctnico on October 07, 2018, 08:24:14 pmThe beauty of technology is that you don't have to worry too much about what's politically acceptable.

author: djacobow
author_rank: Super Contributor
timestamp: October 07, 2018, 09:35:23 pm
content: Though I absolutely agree with the need to tidy up this schematic, I think it supports a thread I started awhile back in the CAD sections which is that fundamentally, schematics kind of suck, particularly for digital circuits. (https://www.eevblog.com/forum/eda/no-schematic-pcb-workflow/)Personally, I hate drawing them and I hate the fiddly time it takes to make them look nice. It's not that I don't see the advantage of them being nice and readable -- I do, and that's why I try to take care. But I just don't like it. Like, for me it's one of the least fun parts of electronics design. I don't mind optimizing a PCB layout, but I do mind "optimizing" a schematic layout.A lot of this work can be reduced through judicious use of hierarchy. If you have "n" of something, draw it exactly once. And do not draw it once and then copy/paste it. Just show it once, too.The example is largely an analog circuit, so I think there's almost no getting away from schematics, but for the digital portions, I think the world needs to move towards something that is text-based, like a netlist format, perhaps with the right macros and syntactic sugar to make it a little less painless. Basically, an HDL but without inferred instantiation (eg, synthesis).I started my career in semiconductors and we moved away from schematics for digital stuff a long time ago. I was honestly surprised to start working on boards and find these huge sheets of chips connected to each other.Just my $0.02

author: Mr. Scram
author_rank: Super Contributor
timestamp: October 07, 2018, 10:35:36 pm
content: Quote from: djacobow on October 07, 2018, 09:35:23 pmFew people like to document their work, which is probably why the documentation tends to be in such a sorry state almost everywhere you look. It's easy to neglect too, because paying the price always comes much later and people generally have actual problems to solve right now.

author: SL4P
author_rank: Super Contributor
timestamp: October 07, 2018, 10:45:02 pm
content: The tedium of drawing a complete schematic isn't rewarded immediately - but one, two, five years later!Damn Scram - you beat me to it!

author: wilfred
author_rank: Super Contributor
timestamp: October 07, 2018, 11:05:52 pm
content: Quote from: EEVblog on October 07, 2018, 02:24:29 pmIt would still get fewer views than Top 10 Halloween ideas for a broken kitchen motion sensor bin. Better make it Top 11.Seriously if you're chasing views you've choosen the wrong niche. This one has 1.3M views and sadly I'm one of them. But only because I saw one on the roadside and was curious about it. I flirted with the idea of having a creepy head pop out as it opened. You're welcome to the idea if you want it.

author: SeoulBigChris
author_rank: Regular Contributor
timestamp: October 07, 2018, 11:47:36 pm
content: Quote from: mikeselectricstuff on October 07, 2018, 08:35:00 pmIndeed. This used to drive me crazy. I called it a visual net list.

author: SeoulBigChris
author_rank: Regular Contributor
timestamp: October 08, 2018, 12:04:27 am
content: Regarding logical vs physical symbols, I came to learn over the years that there can be more than one schematic of the same design. There’s the functional schematic that explains the design itself, using op-amp symbols in this example. This schematic is typically used by engineers.Then one could also prepare a schematic focusing on the physical layout of the printed circuit assembly itself. This type of schematic would be used primarily by service technicians (back when electronics were more serviceable), and would have typical voltages, waveforms, etc. This is where you’d most often use physical symbols like the dual op amp in this example. This type of schematic wouldn’t be prepare unless the product warranted it, which is infrequent in my experience.A couple of other things about kinds of schematics that I’ve picked up...A single assembly might have multiple schematics, not just the functional and physical types. For example, one huge test assembly that item I built years ago involved both electronics and plumbing (compressed nitrogen). In that case, we ended up with an electrical and a piping schematic (which threw a wrench in our company’s drawing numbering system).Last point, which I think may be controversial, is that was taught that the schematic describes the circuit, and the PCB layout describes the physical implementation. This means that if you have two physical versions of an assembly, let’s say a thorough-hole version for lab testing and a surface mount version for production, they would have the same schematics. The different implementations are handled by the BOM / footprint mapping table. This sounds good in theory but often falls apart in practice, so I can’t really disagree with people who insist on a schematic than locks you into a particular physical implementation.

author: tautech
author_rank: Super Contributor
timestamp: October 08, 2018, 12:06:06 am
content: Nice vid Dave, should be a compulsory watch for PCB CAD newbies.A question if I may about the inclusion of component names/values and designators into the schematic symbol.For example, when using 'box' components like resistors and some IC's I place the resistor value into the box and leave the designator outside.IC's I place both into the box. Likewise with say logic gates, only the part # close to U*A and then U*B, C, D etc into the schematic symbol.Good/acceptable practice or not ?

author: SL4P
author_rank: Super Contributor
timestamp: October 08, 2018, 12:21:29 am
content: I’ve worked on some beautifully engineered gear, and the best sets had three major tech docs...— Schematic (detailed)— Block (roadmap to schematic and functionality sometimes with wiring/ loom maps)— Theory of operation (explains the operation of each ‘block.The doc package came as a set of 3-inch thick binders!You could almost repair these $500K / half ton machines without opening the box!

author: SeoulBigChris
author_rank: Regular Contributor
timestamp: October 08, 2018, 02:55:46 am
content: A project leader of mine from way back had one more rule in addition to the “functional flow should go from from left to right”. He insisted that all connectors be isolated on their own sheet, usually sheet one. We griped and groaned about it at the time, but it kind of grew on me. I will do this for a large design, and even in a small one-page design I follow his rule in spirit by showing all connectors along the edges of the page.

author: SeoulBigChris
author_rank: Regular Contributor
timestamp: October 08, 2018, 02:58:52 am
content: I wish the standards for reference designators, symbols, etc., were freely available. Last I checked they were spread around various IEEE and ANSI standards which you had to pay for. I was fortunate to work for a company in my early years that had these documents available, but the cost is kind of steep for the hobbyist.

author: Bud
author_rank: Super Contributor
timestamp: October 08, 2018, 03:06:28 am
content: Quote from: tautech on October 08, 2018, 12:06:06 amYou are not being consistent then, 'cause the other components are annotated differently.

author: grouchobyte
author_rank: Regular Contributor
timestamp: October 08, 2018, 03:15:09 am
content: Quote from: chris_leyson on October 07, 2018, 07:19:23 pmI wholehearted agree with Dave’s pointers vis a vis creating schematics. I too have no set rules but as Dave points out quite clearly, there are certain acceptable standards and there are acceptable exceptions to those norms depending on the design and a bunch of other factors. I am personally a neatness fanatic and have been complimented by hundreds of EE’s that have read my schematics over the past several decades. They may not like or agree with my designs, but they all like the readability and clarity.As far as left to right is concerned, the flow of your schematic should probably depend on whether you are following Hebrew or Sino tradition. One thing for sure, nothing (no I/Os) should enter or leave the top or bottom of a page/sheet@grouchobyte

author: TERRA Operative
author_rank: Super Contributor
timestamp: October 08, 2018, 03:27:12 am
content: Quote from: SeoulBigChris on October 08, 2018, 02:55:46 amToyota schematics do a similar thing.Each connector on the schematic has a reference number, so you can go to the 'connector manual' or sometimes the connector page (if included) in the service manual you are reading the schematic from and see a drawing of that connector with pinouts etc.Makes identifying connectors in a greasy loom down the side of an engine much easier.

author: sibeen
author_rank: Frequent Contributor
timestamp: October 08, 2018, 05:44:49 am
content: I've always liked the connectors on their own page a nice feature.Another that should be added, especially for largish circuits that will be across multiple sheets is that the sheets should have numbers down the side (0 to 9) and letters across the top (A to M) so that when signals jump to another sheet they are given a reference, or when you are looking at the sheet containing the connectors each signal will have a name but also a reference allocation, eg M_RECT [4-M7], signal name is M_RECT and it can be found on sheet 4 location M7.

author: sleemanj
author_rank: Super Contributor
timestamp: October 08, 2018, 06:13:16 am
content: I always find it kind of annoying that schematics rarely have any notes on them. Tool often don't even provide a good way to include notes. A simple note about why a particular value was chosen, or what the intent of some circuitry is, or ... can go a long way to helping yourself when you come back to it 6 months or 6 years later.It's like if you wrote 10000 lines of code, without a single comment. Which, sadly, I also see a lot of :/Also, busses, use busses, don't know how other packages handle it but DipTrace's way works well to make it far tidier and easier to see what goes where than both running lots or wires, or using random floating labels.

author: Mr. Scram
author_rank: Super Contributor
timestamp: October 08, 2018, 06:35:37 am
content: Quote from: sleemanj on October 08, 2018, 06:13:16 amI started a thread about this a while back and the few replies that I got were "there isn't really a standard". As you say, that's very surprising. I sometimes struggle to remember why I made a decision a few weeks later, so there's no chance anyone will know when that's years later or somebody else entirely. Some of us will remember this happening to Keysight, as they were forced to release a public safety warning about a bench multimeter while they scrambled to justify a design choice that wasn't immediately apparent. They damaged their brand and caused issues for their customers simply because they didn't have a note on the why and how.

author: maginnovision
author_rank: Super Contributor
timestamp: October 08, 2018, 07:01:52 am
content: Quote from: mikeselectricstuff on October 07, 2018, 08:35:00 pmOne board I have now has 100 pin CPLD, 144 pin MCU, 50 pin input connector, a bunch of level shifters for all of those 50 lines, audio and video amps. I like to logically separate things across sheets. MCU system(left/right/top power inputs, clock, programming header, reset, internal sys ctrl), MCU IO(Two banks), Power supplies(10V, 5V, 3V3, 1V0), level shifters(56 pin, 3 20 pin, 24 pin), interfacing(display, encoders, buttons, switches). Decoupling capacitors are on the pages for the IC's that use them. Plenty of stuff has connections but for me it would just be a mess having a single page and difficult to follow. Yes you have to switch pages but you don't have 50 lines crossing here and there or make multiple symbols for IC's just so they match for the specific project. I had to choose pins to make the board layout work, so the schematic has to be separated to be readable or possible to follow. It would also be impossible to print in one page. The interfacing page could be combined with MCU IO but it wouldn't be much of a help. I might be bad at this but I can't imagine it be any nicer if all the nets were "physically" connected.

author: sleemanj
author_rank: Super Contributor
timestamp: October 08, 2018, 07:15:36 am
content: Quote from: maginnovision on October 08, 2018, 07:01:52 amUse a bus.Here is a trivial example from diptrace, just imagine it as a far more interesting and pin-involving thing with many modules spread over pages...

author: maginnovision
author_rank: Super Contributor
timestamp: October 08, 2018, 07:31:10 am
content: Quote from: sleemanj on October 08, 2018, 07:15:36 amI'm not sure I see the difference. Instead of pages I connect my logical blocks with 1 line? Eagle busses are also sort of crap. They are basically just lines you draw. It'd be the same effective thing if I just added a note detailing flow, although the pages are already sorted for that.Just to add... Busses in EAGLE are REALLY ugly as well unless I'm really missing something.

author: johnwa
author_rank: Frequent Contributor
timestamp: October 08, 2018, 07:35:00 am
content: Quote from: SL4P on October 07, 2018, 05:30:21 pmYes, or as an extension of this concept, there should be a 'voltage gradient' from the top to the bottom of the schematic. This can make following complex analogue circuitry considerably easier. Of course, sometimes this conflicts with the 'signal flow from left to right' idea, any you will have to choose which one to follow (Think of a common base amplifier for instance).Re angled wires, like GOTOs, these should definitely be used sparingly, but can occasionally make things clearer. The USB data lines in Dave's schematic could have been crossed over this way (although editing the the symbols to make the pins match would be better still.) The traditional two transistor multivibrator is another instance.If I am drawing a schematic by hand, I still like to use the little 'loops' for wires that cross without connecting, which then renders a four-way junction unambiguous. Sadly though I have not come across any schematic software that supports these... But that is really just a matter of style.This was definitely a good topic for a video Dave, hopefully whoever draws the next schematic I have to interpret will watch it!

author: sleemanj
author_rank: Super Contributor
timestamp: October 08, 2018, 07:45:59 am
content: Quote from: maginnovision on October 08, 2018, 07:31:10 amI don't know how Eagle handles it, but as you can see in the screenshot in DipTrace the bus can be split, those two sections of the bus could be on separate pages as long as they have the same name ("ATMEGA") they are the same bus.So imagine that the CP2102 is on a different page, you open that page and you can immediately see that "oh, that connects to RX on the ATMEGA", you don't have to say "that connects to something called RX, now where is that", which if you have a very complicated schematic and you're not familiar with it (any more) might not be such a simple thing.

author: VK3DRB
author_rank: Super Contributor
timestamp: October 08, 2018, 12:02:16 pm
content: What some schematic writers forget is there are two proposes to a schematic:1. To define electrical connections to layout a PCB for example.2. To communicate to humans. That includes debug technicians, or the next poor bunny who has to change the schematic.Back annotating is great but must be treated with caution. It can be valuable to help debug techs locate parts on a PCB, but it back annotating makes no sense during the development process from when the designators are defined in test plans, test results and BOM quotes.Use version control (eg: SVN, GIT or SharePoint), and make sure there is a change history somewhere, either on the top sheet, back sheet, or a separate document. Altium works with SharePoint quite well, and even SVN, but from my experience Altium 18 has too many problem with GIT. Even for beginners, SVN is pretty easy to master. SharePoint is a whole new world of file management thinking.One other point... Use IEEE standard symbols and designators. It make is easier for everyone and avoids painting yourself into the ambiguity corner. Also make rules for your net labels! Eg: nRESET or /RESET or ERROR-FLAG. You cannot use an underscore with Altium because the stupid thing is masked by the wiring - a "feature" that Altium has never bothered fixing.I could write a book on it, but I won't bore you here.

author: maginnovision
author_rank: Super Contributor
timestamp: October 08, 2018, 03:12:11 pm
content: Quote from: sleemanj on October 08, 2018, 07:45:59 amIn eagle it's a graphical element, unless you make custom symbols. If the design were finished we could create custom symbols to make ports that contain all of a set. Those can use busses directly. So far good net names make it clear what is what and where it goes. I'll actually recreate the current schematic though using normal symbols and see how it feels. Then I'll see if it seems clearer to anyone. I'm just one guy so maybe other people hate it and just aren't telling me, other than here.

author: German_EE
author_rank: Super Contributor
timestamp: October 08, 2018, 05:21:43 pm
content: Dave, a minor correction to your schematic. I believe that the section after the AC/DC switch isn't a filter, it's a range switch. 1.1M ohm is 100 times greater than 11K ohm so this switch is used before gain selection on the weirdly drawn op amp. The two capacitors in the circuit are frequency compensation, similar to a scope probe.

author: ANTALIFE
author_rank: Frequent Contributor
timestamp: October 09, 2018, 11:42:57 pm
content: Do you have a link or a number for a good IEEE standard for symbols & designators?

author: rrinker
author_rank: Super Contributor
timestamp: October 10, 2018, 02:17:38 pm
content: Video length when actually teaching something doesn't bother me. I just watched it over 2 sessions.While I have 0 industry experience, I can't imagine making a schematic as horrible as that. I've torn up and redrawn DaveCad-style schematics because I drew myself into a corner and would have had to draw lines all over the place to connect things. here's just no excuse when using a computer program, it's too easy to align things, rotate them to face the same way. etc without needing to completely start over. That's just lazy, not incompetence. I do a lot of network and system diagramming with Visio for my job, and I'm just OCD enough that everything HAS to line up horizontally and vertically or else it just doesn't look right. No weird steps in lines connecting things. I may not draw the most professional schematics for my projects, but my resistors all line up, the wires all come out straight and don't cross through components, and the grounds all face down so the electrons drain properly.

author: Sudo_apt-get_install_yum
author_rank: Regular Contributor
timestamp: October 16, 2018, 08:38:52 am
content: Nice and long video Dave!Does anybody know how to add "grouping frames" to your schematic in eagle? I know Dave is using Altium but I’m wondering if there is a way to do the same in Eagle.Currently I just stick a frame around everything and use different sheets if it’s a more complex design, but I think it would be nice if I have a small design that I just want to group together in "modules".PS: I know Eagle has a new modules function but that not really what I’m looking for.

author: Smokey
author_rank: Super Contributor
timestamp: October 18, 2018, 09:20:38 am
content: I always make the footprint/symbol name visible, especially for passives. If you make the name short and put the package size in the name (ie. R0402 for an 0402 resistor) then it's not much extra clutter and it's super useful for confirming the correct package is used when doing a schematic review.

author: artag
author_rank: Super Contributor
timestamp: November 04, 2018, 01:45:57 pm
content: Quote from: mikeselectricstuff on October 07, 2018, 08:35:00 pmTHIS, in buckets !I guess it's easy to follow the signals if you're in the schematic editor. But if you don't use that same editor and are using a printout or electronic copy, it's utterly useless, especially if you use multiple pages. You can never find where the signal goes and, worst of all, if you find the matching name, you have no idea if it goes more than one place. DON'T EVER DO THIS !Seems like some people aren't trying to draw a schematic. They're just using the schematic editor to create a net list.Well, why bother with the picture ? Just enter the net list as text and save a whole lot of effort.And don't imagine you're created a useful schematic

author: artag
author_rank: Super Contributor
timestamp: November 04, 2018, 01:50:39 pm
content: @CerebusGood point. But while the diff pair is easily recognisable and what I'd tend to use, I really like that alternative you've shown. So much neater without the wire that turns around and goes backwards. I wish that the second form were common enough that it was also instantly recognisable as a standard circuit.

author: Smokey
author_rank: Super Contributor
timestamp: November 04, 2018, 08:22:12 pm
content: Quote from: artag on November 04, 2018, 01:45:57 pmThis is why, in my opinion, Altium Ports are superior to Nets. You can turn on that feature for Ports that shows what pages they are used on. It shows up right next to the port like "2,4,5".

author: Clear as mud
author_rank: Regular Contributor
timestamp: November 06, 2018, 03:16:43 am
content: Someone asked for a link to the technical standards for reference designators and electronic component symbols.IEEE-315is one of them. Also see the references at the end of the Wikipedia articleReference designator.Someone else mentioned that the standards can be expensive for a hobbyist. I found that there wasn't much need for the actual entire standards book. The more common designators are easy to remember, and whenever I'm working with some weird component and I don't know what letter to use for a reference designator, I can just do a web search and usually find some comment or document that tells what the standard designator is.

author: jfitter
author_rank: Contributor
timestamp: March 19, 2019, 07:46:29 am
content: Re the nano wars. This is just my 2c worth, but I have a corporate standard and it is important to pick a standard and stay with it.1. I never use units. A capacitor is in Farads, so why clutter up the schematic with the unit; resistors are in Ohms, etc.2. Multipliers replace decimal points, always.3. Trailing zeros are unnecessary.4. I never use lower case except for comments.Examples;Resistors 100R, 1R5, 10K, 1M, 1M5, 0R002Capacitors 10P, 100N, 100U, 6U8, 2U2, 3N3, 1NInductors 100UThis keeps the drawing clear, legible, and resistant to duplication noise.Of course there are exceptions which can be dreamed up. If you must use M for milliFarads, which I hate, how do you differentiate it from mega. You do it with common sense. If it's a capacitor and your circuit is smaller than a dumpster then it is not megaFarads.

author: eti
author_rank: Super Contributor
timestamp: December 04, 2021, 06:59:56 am
content: Well the designer is certainly a "maker" - he made a real pig's ear of that.

author: Jester
author_rank: Frequent Contributor
timestamp: December 04, 2021, 02:42:42 pm
content: I have “cleaned up” far too many schematics that started out as indecipherable 10 or more pages to just a few pages or even just one large page. The ability to tweak the pin arrangement in Altium easily and have numerous variations of the same component really helps. Yes it takes time up front but the payoff is well worth it in the long run especially if others less familiar with the circuit will rely on it for troubleshooting etc.I also find comments and expected waveforms at critical test points helpful.I prefer to have a well organized and commented (even if congested) single page schematic than having to bounce from page to page to page.For the last 10 years or so I have been relying on different Color’s for digital IC’s (yellow) vs. analog (blue), a specific Color for voltage regulators etc. it helps “paint the picture” of the circuit at a glance when you go back years later. Yes I have a shade of OCD.My 2c