Schematic Drafting Standards - Page 1
Forum section: electronics / projects

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: August 31, 2024, 05:29:07 pm
content: Hello Everyone,I am currently in the process of creating best practices for schematic and PCB layout. There are a couple of great posts regarding this topic on this forum and on Electronics Stack Exchange. Just a few:https://electronics.stackexchange.com/questions/28251/rules-and-guidelines-for-drawing-good-schematicshttps://www.eevblog.com/forum/projects/the-best-schematic-layout-standards/I am about to go into battle with, as a term of endearment, Boomer executives who never had experience with day-to-day engineering tasks and will simply default to "Back in my day 30 years ago...so do it like we did." I would like something more than "read this excellent post by experienced engineers" because that is exactly how they perceive: as an "Internet post."So the pertinent question: is there an IEEE or ANSI standard for electronic schematic drafting standards that I can use as a reference? My Google-Fu has failed me.

author: tggzzz
author_rank: Super Contributor
timestamp: August 31, 2024, 05:44:42 pm
content: Quote from: 16bitanalogue on August 31, 2024, 05:29:07 pmCreate the schematic for the readers' benefit, not for your convenience.Signal flow left to right and top to bottom, except for feedback paths.Use conventional symbols for components, which meansneverhaving a schematic symbol which has all the pins in the same position as the component on the PCB (but do put the pins on the schematic!).Use the standard "design patterns" for subcircuits; that aids rapid comprehension.Don't force fit everything onto one sheet.Use hierarchical diagrams where it aids comprehension.Explicitly connect all components with wires; don't draw an IC, name an otherwise unconnected net, and expect readers to join all the names together. Exception: power supplies. EDIT: group similar signals (e.g. data or addresses) into a bus, and label where they enter/exit the bus. That both "connects all" and "minimises spaghetti clutter".Don't bother to put digital IC decoupling capacitors next to the IC. Do put analogue circuit decoupling capacitors next to the specific IC they are decoupling.

author: exmadscientist
author_rank: Frequent Contributor
timestamp: August 31, 2024, 05:50:37 pm
content: QuoteNope. And where they might exist, they arehopelesslyoutdated or just plain trash.(There are such standards for individual schematicsymbols, and they're pretty decent. But not for schematics as a whole.)Be careful here. This sort of stuff is always a mess, with tons ofbikeshedding. It is generally a big fight. In a previous life I was fortunate enough to work with a senior consultant who shared my mindset, and the two of us were senior enough (and the rest of the engineers apathetic enough, at least about this; note that we only tried this after a certain person left!) that we just forced through a nice set of standards. I still have a copy, and can dig them up (I actually continue to work to this standard where no other rules exist, which is common; it's a good standard!) I could scrub it and send it over, but it's written "by professionals for professionals": it fills in the parts that need filling in, not the obvious bits or the never-any-agreement bits. I'm not willing to post it publicly, though, so it's probably no help to you either way.The most important thing is that the schematic should be filled with lots of explanations. Many places require a "theory of operation" document. My opinion is that, except in rare cases, this should just be written directly on the schematic. (I think this would have been the norm since the beginning if CAD, with its infinite editability, had come about before vellum. Which it didn't.) This makes for schematics dense with words and explanation... explanation placed right where and when you need it. This isamazingfor smaller projects and teams, especially teams of one. It is not as good at larger companies, both practically ("I don't wanna read aschematic, I'm not an electrical engineer"), logistically (three people cannot easily edit one file), bureaucratically ("where is the XZ-808 document? no, you cannot use a schematic as an XZ-508! I don't care if it's one sentence, we can't release without an XZ-508"), and worst of all culturally ("in 1959 we didn't do that, so we're not doing that today!").So... tread carefully.

author: exmadscientist
author_rank: Frequent Contributor
timestamp: August 31, 2024, 06:01:04 pm
content: Quote from: tggzzz on August 31, 2024, 05:44:42 pmHey now! There was that one, one!, time where the IC guys laid out the pinoutperfectly! Once... maybe twice... in all these years... that was a nice project, I miss that part....No, but seriously, never do this. One of my tells for low-quality schematics is when schematic pin arrangement matches the part physical pin arrangement. Nothing good comes of this.(Now Idooften match them in the library editor when I am drawing the symbol, or otherwise match something in the datasheet, whatever is best for easiest cross-checking. I then rearrange them for maximum schematic clarity before finishing the library component.)QuoteI would also say large connectors are an exception. Too many times I see a giant rat's-nest next to a connector and just have to trace wires through it. Trace labels or ports are not good but they are sure as hell better than a rat's-nest.

author: tggzzz
author_rank: Super Contributor
timestamp: August 31, 2024, 06:48:50 pm
content: Quote from: exmadscientist on August 31, 2024, 06:01:04 pmAh, but was the schematic symbol outline merely a rectangle without embellishments. And did the power supply pins need to be shown?QuotePrecisely. I expect that the designer intended that such schematics would be implemented on solderless breadboards. (Caution: rathole ahead!)QuoteDo group similar signals together in a bus, and label wires as they enter/exit from the bus. That satisfies both "connect everything" and "minimise spaghetti".Don't group dissimilar signals in a single bus. Possible exception: bus control signals such as R/W, CS, EN are "similar".

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: August 31, 2024, 07:04:44 pm
content: Quote from: exmadscientist on August 31, 2024, 05:50:37 pmThat stinks. I only found references to schematic symbols myself. The previous posts mentioned drafting standards [for schematics], so I was hoping by chance these actually existed.QuoteI work at a relatively small company. My colleagues and myself have enough experience and pull to argue for a decent set of company standards. I agree that it is always a battle, but as long as we have a good footing to articulate a 'why' and if there is a disagreement follow up with 'what is another solution?'. Those higher-ups will often acquiesce to our view if they cannot present their own reasoned counter-point.QuoteYou can send them to me in an email if you want. I have always had to learn by the seam-of-my-pants, and never had a good mentor for this particular topic. I always refenced what I could and compiled practices off 'The Internet'.QuoteGenerally I think most of this is covered in a User's Guide: theory of operation of the board, schematic, PCB layout in PDF (gross, but what can you do?), trouble shooting tips, etc. But your last comment, that hits home where I am currently residing. It's laughable. Work as in life is a balance, but noteverytopic should be a battle because "We did" or "We did not" so something decades ago. This is true for those who only worked at one company all throughout their career.Overall, excellent advice.

author: SCSKITS
author_rank: Regular Contributor
timestamp: August 31, 2024, 07:10:31 pm
content: With large parts it helps to break up the part into sections, for example with MCUs by GPIO port, regardless of whether the pins are adjacent.I do the same with the banks in EPLDs/FPGAs where possible.

author: coppice
author_rank: Super Contributor
timestamp: August 31, 2024, 07:16:36 pm
content: Quote from: tggzzz on August 31, 2024, 05:44:42 pmThe point you are trying to make is good, but that's a bad way of putting it. Decoupling is usually a bunch of fairly large capacitors providing a generally tame supply rail for many parts, plus a bunch of smaller capacitors close to key parts. Some of those are analogue and some are not. When a decoupling capacitor is intended to be tightly associated with a particular part, draw it that way. When its part of the general decoupling don't visually associate it with any particular part on the schematic.

author: Kim Christensen
author_rank: Super Contributor
timestamp: August 31, 2024, 07:16:58 pm
content: Quote from: 16bitanalogue on August 31, 2024, 07:04:44 pmOne thing I've found very useful when trying to understand complex equipment and circuitry are block diagrams.Detailed text based descriptions are particularly useful if some part of the circuit is unconventional or odd. Not really needed otherwise.Quote from: exmadscientist on August 31, 2024, 05:50:37 pmThanks for that link.

author: Bud
author_rank: Super Contributor
timestamp: August 31, 2024, 07:20:48 pm
content: Quote from: tggzzz link=topic=438577.msg5625317#msg5625317They should be. The reason is there may be No Connect (NC) pins on the package, which are often not shown on the schemaric symbol. If power supply pins are not shown either , you won't know what they are and would need to check the datasheet. This is in general, as there maybe trivial cases like 74 logic where power pins are well known.

author: coppice
author_rank: Super Contributor
timestamp: August 31, 2024, 07:29:51 pm
content: Quote from: Bud on August 31, 2024, 07:20:48 pmIn the heyday of the 74 family showing the supply pins didn't make sense, especially since most of them contained multiple copies of a functional block, which at the initial schematic level were not bundled. The bundling happened through back-propagation after PCB layout. This has largely gone away, as chip complexity has increased. We are now in an era where there is no standardisation of power pins across a range of parts, a huge number of parts have multiple power rails, and the whole issue of the power flowing to a chip is far more complex. A schematic needs to tell you what is really going on with the power.

author: tggzzz
author_rank: Super Contributor
timestamp: August 31, 2024, 07:47:36 pm
content: Quote from: Bud on August 31, 2024, 07:20:48 pmThat response ignores the context in which my comment was made. Please just use the "quote" button and don't remove too much context.Of coursethe power supply pins have to be shownsomewhereon the schematic. If they aren't then they wont be in the netlist and won't be on the PCB!

author: tggzzz
author_rank: Super Contributor
timestamp: August 31, 2024, 07:49:07 pm
content: Quote from: coppice on August 31, 2024, 07:29:51 pmAgreed.Whether such PSU pins should be clumped together on a separate "PSU schematic", or intermixed with signals is not something with a single correct answer. Good taste is the key, in conjunction with "what makes it easiest for a new reader to understandwhatis intended, andwhy".Note that Bud's comment represents a strawman argument (it snips the relevant context in which I made my statement).

author: tggzzz
author_rank: Super Contributor
timestamp: August 31, 2024, 07:56:30 pm
content: Quote from: 16bitanalogue on August 31, 2024, 07:04:44 pmIf that's the case, why not just agree amongst yourselves?What islostbynothaving a company standard?

author: aeg
author_rank: Regular Contributor
timestamp: September 01, 2024, 05:29:39 am
content: See also "how to draw schematic diagrams" in Horowitz & Hill - The Art of Electronics, appendix B in the third edition or appendix E in the second edition.

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: September 01, 2024, 06:13:24 pm
content: Quote from: tggzzz on August 31, 2024, 07:56:30 pmAs the team grows there needs to be a sense of uniformity. Generally:1. Always do a, b, c2. Never do x, y, z3. Use judgement for 1, 2, 3It's a small company where the executives for the first time in decades are very close to the day-to-day; however, they try to enforce outdated methodology with documentation, process, and engineering methods that they used when they were individual contributors back when Marty was driving 88 MPH.Quote from: aeg on September 01, 2024, 05:29:39 amI have the second edition on by bookshelf. I will include this!

author: tggzzz
author_rank: Super Contributor
timestamp: September 01, 2024, 06:42:58 pm
content: Quote from: 16bitanalogue on September 01, 2024, 06:13:24 pmObvious point: check you agree with what they say! Nobody is above critical appraisalISTR seeing some of their schematics with with everything crammed into one schematic

author: Marco
author_rank: Super Contributor
timestamp: September 01, 2024, 07:13:59 pm
content: Quote from: tggzzz on August 31, 2024, 05:44:42 pmExcept for opamps, everyone flips those over.

author: tggzzz
author_rank: Super Contributor
timestamp: September 01, 2024, 07:31:10 pm
content: Quote from: Marco on September 01, 2024, 07:13:59 pm?yeht oDI don't understand what you mean by that, in that context.

author: nctnico
author_rank: Super Contributor
timestamp: September 01, 2024, 08:35:04 pm
content: Quote from: exmadscientist on August 31, 2024, 06:01:04 pmWell, I assume you never debugged / verified a circuit then. In reality it greatly depends on the part whether it is feasible to draw the part like it is in the schematic. If you can, do draw the part as it is. When doing debugging / verification, all you need to know where to place a probe is the schematic and no need to count pins as you can tell by the external arrangement of the components which pin is which in many cases. This saves a lot of time (which equals money).Another good reason to draw a part in its physical form is that you have a good overview whether all pins have been assigned.Actually, if the schematic looks like a mess when you draw a part in its physical form, the part is likely going to be a nightmare to get routed on the board anyway. So this is a good first sign of how difficult the board layout is going to be. Maybe a different part is more suitable.

author: nctnico
author_rank: Super Contributor
timestamp: September 01, 2024, 08:39:46 pm
content: Quote from: tggzzz on August 31, 2024, 07:47:36 pmThis is not how it used to work in the old days. Many 74 and CMOS series logic libraries still have hidden power pins which are not shown on the schematic anywhere. These are silently tied to net names like VCC, VEE, GND, VSS, etc. which are then automatically connected in the netlist. This is nice and dandy when your circuit only has / needs a 5V 300A power supply but those days are long gone.

author: coppice
author_rank: Super Contributor
timestamp: September 01, 2024, 08:56:35 pm
content: Quote from: nctnico on September 01, 2024, 08:39:46 pmPins obscured on the schematic were always a PITA. Most of the time older chips had the supply pins in very predictable places, but when they didn't you could end up digged out data sheets, checking packaging options, etc, trying to find where the power should be when debugging.

author: nfmax
author_rank: Super Contributor
timestamp: September 01, 2024, 09:17:07 pm
content: Quote from: nctnico on September 01, 2024, 08:35:04 pmAnother approach is to put a package outline, with appropriate PIN numbers e.g. at the corners, as a schematic “comment”. This works for some packages, but not for others like BGA. Comments on circuit diagrams can help a lot

author: tggzzz
author_rank: Super Contributor
timestamp: September 01, 2024, 09:35:02 pm
content: Quote from: nctnico on September 01, 2024, 08:35:04 pmAbsolutely not! What on earth does "draw the part as it is" mean?!The purpose of the schematic is to expose thedesign. That guides understanding what you should observe when you place a probe on a component.The PCB isoneimplementationof the design, and purpose of the PCB component overlay is to expose the components on the PCB.The logical conclusion of your contention is to omit the schematic and use only the PCB component overlay. After all, all you need to do is know which point to probe - don't you? (Hint: no!)

author: tggzzz
author_rank: Super Contributor
timestamp: September 01, 2024, 09:38:37 pm
content: Quote from: nfmax on September 01, 2024, 09:17:07 pmI've never seen that, but that contention holds water.Comments can be overdone and underdone. Good taste is required, and in this context good taste is whatever helps a person trying to understand the schematic.

author: nctnico
author_rank: Super Contributor
timestamp: September 01, 2024, 09:45:28 pm
content: Quote from: tggzzz on September 01, 2024, 09:35:02 pmYes, the purpose of the schematic is to lead to something which is useful. And hence you grossly glossed over the 'it depends' part and the part based on very extensive hands-on experience that -if possible- drawing a part like it sits on a PCB is super immensly helpful to make a schematic actually useful. You seem to keep on wanting to create schematics like abstract art which at some point nobody understands. I for one don't want to be like Picasso in his abstract period; I want people to understand and use my schematics without needing any other documentation as much as possible. This all starts by very carefully choosing how to represent parts in a schematic. But also adding notes, expected voltages, etc. And for more complex circuits things like a block diagram, power-trees, power sequencing, power usages, currents, etc.

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: September 01, 2024, 10:26:53 pm
content: Quote from: nctnico on September 01, 2024, 09:45:28 pmI could see a schematic symbol matching the physical component pins if it were a simple design. I'll confess, I rarely do this and I draw all my schematics from a circuit design oriented point of view. Input/Outputs flow right to left, High/Low voltage from high to low. An op-amp in an SOIC, MSOP, DIP, etc. looks like a triangle. If I really want to mess with people, the old trianglish symbol from back in the day.Pins have their name and number on the schematic. Pins should have associated test points on the PCB. If there is a time that I truly need to measure a pin on a QFN package with a wettable flank, then I will have to pull out the datasheet. Besides, JEDEC standard for QFN packages is pin 1 is top left.

author: nctnico
author_rank: Super Contributor
timestamp: September 01, 2024, 10:34:21 pm
content: I get that, but avoiding needing the datasheet gives you a massive boost in debugging speed and less clutter on your desk / screen. And no, you can't have test pins for everything. A PCB would become a total mess like that AND you can't really predict which test points you actually need for debugging / design verification as surprises may linger.

author: 16bitanalogue
author_rank: Regular Contributor
timestamp: September 01, 2024, 10:40:00 pm
content: Quote from: nctnico on September 01, 2024, 10:34:21 pmMy standard practice is to always have the datasheet on hand; either a softcopy or a hardcopy. This is how I train engineers because it was beaten into me in the bygone days. I am not an expert on every product either, so it has always been a benefit to me to have the datasheet ready to go. Hell, I don't remember every single characteristic of the datasheets I authored myself.

author: nctnico
author_rank: Super Contributor
timestamp: September 01, 2024, 10:45:17 pm
content: That method falls apart if you need to lookup the pinout of every multi-legged part on a board. Also, the purpose of a schematic is that you have an idea of what a signal should look like. In a good schematic even more so than in a datasheet! If a signal name is 'SPI_SCLK' you know you are looking for a clock on an SPI bus. There is no need to lookup the pin function. However, if only there is an easy way to identify which pin to poke... Hence the preference to draw parts as they are layout physically. Again, this is not possible for all parts but it is mighty handy when it is. Think of a simple linear voltage regulator for example. There is no real standard for the pin order on those things. When drawn as they are, measuring voltages on a board gets super easy without needing anything else than the schematic.

author: Kim Christensen
author_rank: Super Contributor
timestamp: September 01, 2024, 11:22:24 pm
content: If you want to see well written manuals, take a look at theolder HP ones written by boomers.

author: tggzzz
author_rank: Super Contributor
timestamp: September 02, 2024, 08:48:19 am
content: Quote from: Kim Christensen on September 01, 2024, 11:22:24 pmI'm not sure what "boomers" have to do with it. Competent engineers in a good company, yes.Nctnico wouldn't approve, though. Those components don't look like what you see on a PCB. Presumably he would prefer (caution ascii art ahead!)Code:-----------| C B E |-- Q1---------|-----------| |-- R1-----------/ \----\ +/---- C1 for a radial mount electrolytic--Personally I get that information from a different type of diagram, like this...

author: tggzzz
author_rank: Super Contributor
timestamp: September 02, 2024, 08:55:41 am
content: Quote from: 16bitanalogue on September 01, 2024, 10:26:53 pmI can't.Too often you see a schematic that looks like a solderless breadboard, with "please help my circuit doesn't work". You can't even tell if theintended designis correct, because who the hell knows which pin is the output/reset/discharge/etc on a 555! Just draw the effin schematic so that it vaguely resembles something seen in an application note.No, I'm not going waste my life on the equivalent of dissasembling optimised object code back into C actually thatistoo strong with microwave circuits; e.g. consider a ratrace coupler

author: Marco
author_rank: Super Contributor
timestamp: September 02, 2024, 10:56:03 am
content: Quote from: tggzzz on September 01, 2024, 07:31:10 pmThe way industry handles opamps in schematics is convenient for absolutely no one.Is inverting on top for inverting amplifiers only? Does the V+ go on top/bottom with non inverting input? Flip a coin for every bit of software, datasheet and schematic. Even in a single datasheet you will find the isolated symbol randomly flipped.

author: tggzzz
author_rank: Super Contributor
timestamp: September 02, 2024, 11:17:31 am
content: Quote from: Marco on September 02, 2024, 10:56:03 amClearly it is convenient for most people, and following standard "design patterns" is A Good Thing in both hardware and software.QuoteFollow the standard design patterns seen in (decent) textbooks and application notes and schematics - unless you want to needlessly make it difficult for other people to understand the design.Positive PSU voltages at the top, negative PSU voltages at the bottom, 0V in the middle.For an inverting opamp circuit, the noninv input is connected to ground, and is therefore more neatly put below the inv input.QuoteNo, you don't see that bad practice is everywhere.Data sheets aren't circuits, and over time are containing less useful information. That's poor.Just because you can see bad practice in some cases doesn't mean you have to loweryourstandards.The OP is interested, sensibly, in good practice, not copying bad practices.

author: Marco
author_rank: Super Contributor
timestamp: September 02, 2024, 11:35:14 am
content: Quote from: tggzzz on September 02, 2024, 11:17:31 amFor a non inverting opamp with a divider to ground it's the other way round ... but unless you have two separate symbols, or symbols without power, you have to compromise.With a single symbol with power compromise which way? Flip a coin if you prioritize the neatness of the schematic or the orientation of the power, then flip a coin again based on your mood.Also major software programs do disagree on which side V+/V- goes.

author: tggzzz
author_rank: Super Contributor
timestamp: September 02, 2024, 11:55:59 am
content: Quote from: Marco on September 02, 2024, 11:35:14 amYou are going to have to learn how to make your own symbols for components that aren't in a library. For something common and simple like an op amp, multiple symbols are usually available. If not, make your own symbol starting from an existing symbol. It isn't difficult, doesn't take long.Having the traditional symbol demonstrates to other people that you take pride and care in your work, and that you understand the circuit's operation. But maybe that doesn't matter to you?By "Major software programs", do you mean CAD program? No library - software, analogue hardware, digital hardware, RF, microwave, music, paper book, etc - is going to contain everything you might possibly need. Learn to use your tools.

author: Marco
author_rank: Super Contributor
timestamp: September 02, 2024, 12:25:37 pm
content: The problem is not whether the symbols are present in the libraries of major software programs with schematic capture like say Eagle or Pspice, the problem is that there is only 1 symbol in each library AND they can't agree what to put on the top and bottom of the symbol (top and bottom being sides of course).The software can't agree, designers can't agree and somehow I doubt even you add a new symbol every time the power connections and input connections aren't perfect for both neatness and consistency of power orientation.PS. I think consistency of the inputs is generally more important than neatness, consistency has value of its own. Except for extreme cases like say three opamp instrumentation amplifiers. Otherwise, I'd rather everyone would pick a side and stick with it (and I'd prefer non inverting on top, but that seems a minority point of view).

author: Kim Christensen
author_rank: Super Contributor
timestamp: September 02, 2024, 03:06:00 pm
content: Quote from: tggzzz on September 02, 2024, 08:48:19 amI was just pulling the OP's chain:Quote from: 16bitanalogue on August 31, 2024, 05:29:07 pmQuote from: 16bitanalogue on September 01, 2024, 06:13:24 pm

author: tggzzz
author_rank: Super Contributor
timestamp: September 02, 2024, 03:46:04 pm
content: Quote from: Marco on September 02, 2024, 12:25:37 pmThe softwareshould NOT"agree" - because it is an electronic design issue. The software shouldenablewhatever is best for the designer, both at the schematic and PCB level. I suppose you also complain that there isn't a single pad pattern for 0603 SMD components. There shouldn't be, since the optimal pattern is a function of component manufacturer and PCB production process.The quality of libraries is (arguably) the key consideration when choosing any software/hardware language or CAD/RF tool etc. Ideally the library will already contain what you need, but inevitably they won't. In that case they should enable you to easily implement your own component.I suggest you look at some different CAD tools and/or learn how to use all their capabilities.QuoteNo.Easy fast comprehensibility is the most important attribute that a schematic should have. Consistency of representation corresponding to industry standard design patterns is key to that.Example: you normally draw transistors in a different orientation depending on whether they are acting as CB/CB/CC/cascode/diff pair amplifiers, current mirrors etc. And that reallyreallyshould not depend on whether the components pins are BCE, CBE, BECase, or anything else.

author: tggzzz
author_rank: Super Contributor
timestamp: September 02, 2024, 03:46:57 pm
content: Quote from: Kim Christensen on September 02, 2024, 03:06:00 pmOK(I did consider the possibility, but didn't want to presume that was the case. Honestly!)

author: Marco
author_rank: Super Contributor
timestamp: September 02, 2024, 04:23:52 pm
content: Quote from: tggzzz on September 02, 2024, 03:46:04 pmWhat consistency? Inverted power connections on schematics are incredibly common ... and I still doubt you actually make new symbols every time to avoid it.My suggestion has the advantage in that it can actually be consistent, without needing two separate symbols.

author: nctnico
author_rank: Super Contributor
timestamp: September 02, 2024, 04:33:06 pm
content: Quote from: Kim Christensen on September 01, 2024, 11:22:24 pmThat template leaves a lot to be desired by today's standards. The part number for the transistor is missing for example. And with a much greater mix of components nowadays, I very much prefer to have complete part numbers (so you can enter the part number in Google and get the datasheet without needing to look at the BOM) and more information about the components. Like voltage rating & package size for SMD capacitors, tolerance & package size for resistors and current rating + DC resistance for inductors. All this information helps to give a good sense of what a circuit is supposed to do and also allows for a quick check on whether the voltage & current ratings are suitable.

author: coppice
author_rank: Super Contributor
timestamp: September 02, 2024, 04:37:36 pm
content: Quote from: nctnico on September 02, 2024, 04:33:06 pmIf an HP schematic gives a part number its usually just an 8 digit HP code, so its not that meaningful to most viewers. Their manuals have a part code to part number table for every schematic, so its easy to find the part you might need to order, but the use of internal 8 digit codes for every part in their products means its not very helpful to have them on the schematics.

author: nctnico
author_rank: Super Contributor
timestamp: September 02, 2024, 05:07:47 pm
content: Quote from: coppice on September 02, 2024, 04:37:36 pmTrue, but for general use, it is highly recommended to have a meaningful partnumber next to the symbol. And with the way modern CAD packages work (especially decent ones which have the components defined through a database), it is much easier to update a part number is a schematic compared to the old days where updating the part number would mean modifying the circuit diagram or re-drawing it manually.

author: TimFox
author_rank: Super Contributor
timestamp: September 02, 2024, 05:10:22 pm
content: That era of -hp- schematics used TH components, rather than SM.It allowed editing of text-file BOMs when, for example, the resistor values were rationalized to use fewer discrete values, although it is helpful to have the resistance value on the schematic.A full listing of parameters for a resistor would clog up the schematic drawing, but could be given on the BOM.Note that the full part reference for the resistor adds the board reference: A2R1 for R1.

author: exmadscientist
author_rank: Frequent Contributor
timestamp: September 04, 2024, 12:11:03 am
content: Quote from: Marco on September 02, 2024, 04:23:52 pmI do. I absolutely, 100%, do it. To be fair, I make extensive uses of Altium database thingies, so I don't have to do it veryoften... but I do it.If I did not do it, my schematics would be hard to read. Quality of my work product is a major factor in why my employer gets to charge $$$ for my time as a consultant, and legibility is the most important part of quality. I have seen many, many different schematics in my career, from multibillion-dollar-company offshored-onshored-reshored-deshored-meshored hot potatoes, to that guy in his garage who barely managed to plug in an Arduino without killing himself, burning down his house, or killing himself by burning down his house, and the common denominator is clear: you are most likely to find solid engineering when the schematic is immediately clear and easy to read.No stupid 64-pin microcontrollers showing pins 1 to 64 in order around a big square component.... (Anyone who thinks that's OK, have you evenseena BGA? How do you thinkthatis supposed to work. It doesn't. Get good at making a 400-ball BGA with eight bloody power rails clear and you will have someopinionson people who think square-box parts are legible.)

author: tggzzz
author_rank: Super Contributor
timestamp: September 04, 2024, 12:23:27 am
content: Quote from: exmadscientist on September 04, 2024, 12:11:03 amYes indeed.The need is especially obvious with FPGAs where there cannot be an existing symbol.Mutating non-rectangular boxes can be a bit tedious, but it is part of pride in avoiding unnecessarily obtuse documentation. And, of course, helping me explain the circuit to myself

author: Marco
author_rank: Super Contributor
timestamp: September 04, 2024, 05:54:29 am
content: Quote from: exmadscientist on September 04, 2024, 12:11:03 amThat's a strange thing to say within the context of that discussion.I'm not talking about big square boxes with "stupid 64-pin microcontrollers showing pins 1 to 64 in order " ... I'm talking about a very specific case, which the whole industry specifically doesn't care much about. Specifically, making an extra symbol for opamps the first time you want to flip it vertically. Altium doesn't help you there, it gives you one symbol with the inverting input and positive supply on a specific side (flipped from a lot of other major software, because as I said, there is no consistency).I didn't want to make a long discussion about it, but I'm not going to be told it's my imagination. I suspect some people are just so accustomed with the lack of consistency, they think inconsistency is consistent. There is no consistencyright down to the software.

author: tggzzz
author_rank: Super Contributor
timestamp: September 04, 2024, 08:21:14 am
content: Quote from: Marco on September 04, 2024, 05:54:29 amThe problem is that you are focussing exclusively on one form of consistency: which pixels are black. Other people are focussing on a different (more useful IMNSHO) form of consistency: how to make the design more easily understood.

author: Marco
author_rank: Super Contributor
timestamp: September 04, 2024, 08:48:05 am
content: Other people not including the industry making schematic capture software, because it's a fact they can't even agree how to put the symbols in the libraries.A debate about the desirability of how I'd prefer to consistently do it is completely orthogonal from the fact that the industry as a whole has absolutely no consistency. Not the software and not the users either.It's most definetely not common practice to make a new symbol for every opamp you use, just so you can simultaneously let the signals flow neatly and have V+/V- top/bottom.

author: tggzzz
author_rank: Super Contributor
timestamp: September 04, 2024, 09:09:49 am
content: Quote from: Marco on September 04, 2024, 08:48:05 amThat point was addressed earlier. TLDR: CAD companiesshouldn't, because only the circuitdesignerknows how to make theirdesigncomprehensibleto other people.QuoteJust because some users emit crap hardware or software designs/documentation doesn't mean nobody should.Strive to be better than average!

author: Marco
author_rank: Super Contributor
timestamp: September 04, 2024, 09:34:16 am
content: Of course the software should have a consistent standard for the default symbols, the users make "extensive uses of Altium database thingies" after all.If the libraries were at least consistent, then the schematics from the lazy users would be more consistent too. Instead it's coin flips down the line.

author: tggzzz
author_rank: Super Contributor
timestamp: September 04, 2024, 09:58:19 am
content: Quote from: Marco on September 04, 2024, 09:34:16 amLet's be clear: you think (ease of) understanding is less important than your preferred form of consistency. I disagree.As Ralph Waldo Emerson memorably put it in 1841, "a foolish consistency is the hobgoblin of little minds".

author: Marco
author_rank: Super Contributor
timestamp: September 04, 2024, 10:39:33 am
content: Quote from: tggzzz on September 04, 2024, 09:58:19 amI have factual knowledge of my thoughts and I can quite objectively say you are wrong.Why turn the factual observation of complete lack of consistency in the tooling and industry users into a discussion of my mindset though?