Which CAD package produces the best looking schematic and why - Page 1
Forum section: electronics / general

author: DIPLover
author_rank: Regular Contributor
timestamp: January 21, 2015, 09:44:46 pm
content: When looking at books from the 80's and early 90's, I am often amazed by the quality of the schematics they contain. They just look so sharp with fine lines and well routed bus lines and perfect part symbols...An example book whose schematics I have tried (and failed) to emulate is "68000 microcomputer design" by Alan D. Wilcox.I do not know what tools (if any) where in general use then, but I find schematics from Altium, Eagle and Diptrace to be ... unrefined?Is schematic entry/capture now only a means to accelerate PCB development?Does anybody still care?What is your favourite schematics drawing package and why?Any books you would recommend for improving schematic drafting (or just looking at great examples) ?

author: nctnico
author_rank: Super Contributor
timestamp: January 21, 2015, 09:49:41 pm
content: I still like the way Orcad Capture prints a schematic either in color or black&white.I don't like Altium because Altium prints on a shaded background which makes a diagram hard to read when printed in black&white. Also the font (Times) used is really hard to read. The last time I used Altium I have not been able to change the font used for the parts and wire labels.

author: c4757p
author_rank: Super Contributor
timestamp: January 21, 2015, 10:06:14 pm
content: Most packagescanproduce a decent schematic if you put in the effort. Here's an example from a schematic I'm working on now - okay, the arrangement of the schematic isn't perfect - still a work in progress - but here are the general component symbols I use and the text style of the software. I think it looks quite nice, and the general styling is reminiscent of that older schematic style.FWIW, I like the look of Altium schematics, including the font.

author: DIPLover
author_rank: Regular Contributor
timestamp: January 21, 2015, 10:15:20 pm
content: I will try to scan a small example when I get back home to illustrate my point, this is all very subjective of course.

author: ajb
author_rank: Super Contributor
timestamp: January 21, 2015, 10:38:23 pm
content: We typically thing of drawing schematics as engineer's work, but as a form of technical drawing it's as much graphic design as engineering. So it helps to look at it with a designer's eye. A lot of it I think comes down to establishing a style and making your schematic library conform to it. Things like line weights, scale, and shape are important here, and putting some time into simply making all of your symbols look like they belong together on a page will go a long way towards making your schematics look better. Unfortunately many EDA programs have very rudimentary graphic capabilities (I'm looking at you, Altium, with your TERRIBLE arc tool!) that can make this tricky.I think a lot of what makes older schematics look so nice is that they were drawn for black and white. When you can't lean on color to differentiate objects, you have to pay a lot more attention to lines and layout. At some point I think I'm going to convert my Altium library to mainly monochrome for exactly this reason.Other than that, CAD makes it much easier to tweak (or completely rearrange!) your schematic at any point in the design process, so it helps to simply take a step back and look at your schematic and ask yourself things like:- Is the flow of power/information through the circuit clear?- Are the most important functional elements visually apparent, or are they hidden amongst peripheral parts?- Is the schematic pleasing to the eye, or does it look like a big jumbled mess? That sounds like a purely aesthetic question, but it's a good gut check for legibility.And then revise accordingly.

author: free_electron
author_rank: Super Contributor
timestamp: January 21, 2015, 11:25:31 pm
content: that's what i do. my library symbols are monochrome only. i try to follow iec standard for the symbolsintegrated circuits are always customized in my case to untangle spaghetti.netnames are only used inside the same page, ports go off page.a wire always connects two points. no stubs with a netname slapped on going nowhere. it either goes in a bus or on a component.don't overdo annotation. too much text is an eyesoreresistors : value and tolerancecaps : value and voltagei now modded my cap and resistor symbols to have a marker inside that tells you if its 0402 0603 0805 etc.i no longer uses fixed comments but set them dynamically to parameters in the parameter list. caps have parameters added like value ,voltage, dielectric. resistors have parameters called value, wattage, tolerancethis lets me pull very clean assembly data in the bom outputkeep everything standard line thickness. use sans serif fontand what is this 'terrible arc tool' i hear about in altium. it's perfect. draw arc , manipulate endpoints and origin. done. you;re probably doing it wrong ... please explain what makes it horrible.

author: Rigby
author_rank: Super Contributor
timestamp: January 22, 2015, 12:13:34 am
content: Quote from: c4757p on January 21, 2015, 10:06:14 pmLove it.Mergenthaler had some equipment back in the day that made schematics meant for printing.Check this video:

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 22, 2015, 01:23:53 am
content: Quote from: DIPLover on January 21, 2015, 09:44:46 pmWhen it comes to print: who knows. Tektronix used by-hand draftsmen for decades, and that was not only good enough for them -- it was arguably a distinctive feature among test equipment manufacturers.As mentioned, the Diagrammer certainly would've been useful to some, but who knows what else would've been available, and to what level?It's possible to make nice drawings in Altium, Multisim (a challenge), Eagle (which I don't use, but I've seen a few reasonable examples of) and so on.I've heard good about xcircuit.There's also a LaTeX package, which I don't know how well it works for executing layout (I haven't tried it), but you can just imagine the power that can offer, if done well.QuoteWell...Bleh...The average engineer these days, it seems to me, imagines themselves as in opposition to their subject, as though creating designs is a sheer act of will and defiance, of forcing ones' analog mind into the digital and the graphical (here by 'graph', I mean abstract graph theory: the connection of nodes in a circuit). My justification for this assertion is, so many commercial designs are UGLY, if you ever get to see the internal drawings they use. File names are often written in 8 letter ALLCAPS as if it's still the 1970s, or with underscores as if machines can't handle spaces today. It's as if the designers perceive an abstract computational will, that everything should be made difficult to use, because it is difficult to them!Some examples of ugly schematics:- Excessive use of Net Labels- Discombobulated, everything spread out; no high level structure- Everything on a single sheet /- Everything on a separate sheet!- Components, lines, labels, etc. not drawn on grid (sometimes resulting in connectivity errors, especially during maintenance of the design!)- Components, labels, etc. rotated or positioned in stupid locations (labels overlapping components, pins, other labels, etc.; components not obeying the "vertical to supplies - signals across" rules)- Everything just in terrible proportion, if any at all. No balance. No sense of aesthetic.QuoteI do good work in Altium, or I like to think so; which brings this point,Quote from: nctnico on January 21, 2015, 09:49:41 pmCheck the Document Properties, or edit the Template; the document background color can be changed.Whoever decided to make it an off-white cream color should be shot.Labels can be changed (en masse if you like) by selecting them and editing the Font property in the SCH Inspector.Full project example:- Open all schematics- SCH Filter Panel, select "from all documents in project", query "IsDesignator OR IsComment" (or something like that -- I forget offhand which one it is, because some OTHER retard had the wonderful idea to call schematic designators and comments a different primitive (Is object) from the respective objects on the PCB, argh!)- SCH Inspector Panel, select "from all documents in project" again, change font.- Optional: Shift+C to deselect all components in all sheets, so you don't accidentally change one object on the current sheet PLUS all the others still selected off screen. D'OH!Or SCH List Panel, "from all documents in project", select object types for labels and all that, sort by Visible, and now you can play with all the labels or attributes that are visible, not just designators and comments.Anyway, Altium aside; I try to draw things nicely. So, here's a snippet I drew in Altium some long time ago,this is just a screenshot, but still, notice the positioning and orientation of components, labels and so on. I also redrew several components, because the library symbols are capital UGLY.My schematics are drawn much the same in my old standby, Paint:where of course all the symbols have been hand crafted, rather than pulled from library. So they meet my preferences, of course. Major downside: designators are horrible to edit, so I tend to be lazy and leave them off (and eventually forget some anyway... oh, wait...).Here's a good example of trash that's easy to make in Multisim:http://seventransistorlabs.com/Class_D_Amp.pdfI (much later) cleaned this up by hand,http://seventransistorlabs.com/ClassD1/Images/ClassD_Full.pngMultisim is a pretty crusty environment so it took me a long time to figure out how to make actually presentable schematics there. Routing, orientation and proportion always apply, of course. Hint: you can nudge text labels by selecting them and using the arrow keys. This allows you to (manually) fix their positions, which often end up in stupid places (e.g., Q6). The default labels can also be disabled (on the part property dialog, second tab), say to get rid of all those damn "TEST_PT1" comments are are useless.Biggest advice for the newbies:Take the time to make something presentable!Not only will you end up with something that the experts can answer more quickly, you'll better understand the circuit yourself just by redrawing and rearranging it.Turn off default labels, or assign them useful values. We WILL read the labels on the schematic, because we can only assume you meant to write everything that you illustrate! Pick values and components thoughtfully. Fill out part numbers, so we can get some idea of where you're going with things -- don't leave generics unless you're absolutely sure that a generic really truly is generic (if you're a newbie, you probably aren't experienced enough yet to determine that -- so please do be as specific as possible!).Don't provide a jumble of components, with default designators, and unspecified values, and expect us to deal with your mess!Tim

author: Richard Crowley
author_rank: Super Contributor
timestamp: January 22, 2015, 01:35:46 am
content: The benchmark for beautiful schematic diagrams was Popular Electronics magazine which I read faithfully growing up.They are still unequaled in modern times, IMHO. The proportions of component sizes, typography, etc were perfect.You can see the entire lifespan of the publication online:http://www.americanradiohistory.com/Popular-Electronics-Guide.htmMeanwhile at the opposite end of the spectrum (and in the same historical era), the service manuals for IBM mainframes wereEBCDIC "printer art" on huge line-printer pages. Very remarkably crude and nearly unreadable except to an experienced IBM service-man.Maybe you had to be wearing a long-sleeve white dress shirt and a proper IBM neck-tie to properly read those old things.Here, someone has re-purposed one of the wire carts made for those huge binders, and put regular A-size binders in the slots...

author: Rigby
author_rank: Super Contributor
timestamp: January 22, 2015, 02:25:58 am
content: Those look a lot like old Wells-Gardner schematics from a few years back.http://www.wellsgardner.com/pdf/Service/K7000.pdfNot perfect, optimized for size and not clarity, but the symbols are perfect, IMHO.

author: DIPLover
author_rank: Regular Contributor
timestamp: January 22, 2015, 02:43:24 am
content: Here are some (bad) scans from the book to serve as examples of what I like.I like :- The symbols- The fonts- the designators inside the symbol- the symbols on the bus drivers- the main ICs sized to fit the surrounding components- the "overall view" and left to right "flow"- the sheet connectors on the 68k schematic- the omission of pin designators inside the 68k symbol since ALL signals are named on the bus lines makes it much cleaner.- the little notes spread around the interesting bits.Theres also some intangible aesthetic quality I can't quite name.I'd like to make my schematics like those, but my tools seem so crude...

author: Rigby
author_rank: Super Contributor
timestamp: January 22, 2015, 02:46:35 am
content: Inkscape or Illustrator could produce these, almost certainly.

author: c4757p
author_rank: Super Contributor
timestamp: January 22, 2015, 02:49:21 am
content: I like this style - might modify a bit of my library according to some of it.There are a few WTFs though - what on earth were they thinking with this completely unlabeled 555, for instance?!And this is definitely something that just about any program can do. Helps to have "parts" in the library to quickly add some of the nice annotations, like the arrows specifying drive direction to/from the bus, the little waveform symbols, etc.

author: DIPLover
author_rank: Regular Contributor
timestamp: January 22, 2015, 02:51:15 am
content: Quote from: Rigby on January 22, 2015, 02:46:35 amUndoubtedly but I'd like to do them as CAD drawings, to get a netlist and all that, not just as illustrations.

author: DIPLover
author_rank: Regular Contributor
timestamp: January 22, 2015, 02:52:45 am
content: Quote from: c4757p on January 22, 2015, 02:49:21 amThe 555 used for power-up reset pulse is explained in details and has its own full page schematic elsewhere.Also a 555 in 1987 might not have needed so much explanation... Weren't they building EVERYTHING out of those for years already?It's hard to find a single diagram that really explains why I like his style so much...

author: DIPLover
author_rank: Regular Contributor
timestamp: January 22, 2015, 03:10:02 am
content: As a comparison point, here is a little work in progress from Diptrace (which I think is a mighty fine program for the price).There is a LOT of work still to do but notice the ugly fonts, and very LARGE passive elements (resistors etc.). Why are these things so big?The Canned oscillator as a sweet default symbol though.Why am I jealous of a 27 years old diagram?

author: c4757p
author_rank: Super Contributor
timestamp: January 22, 2015, 03:36:34 am
content: Quote from: DIPLover on January 22, 2015, 03:10:02 amThis is my single biggest (and possibly weirdest) schematic library pet peeve.icicicdiodeicictransistordiodeRESISTOR!!!!!!!icicicdiodetransistoricCAPACITOR!!!!!!!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 22, 2015, 04:00:41 am
content: I'd prefer bigger diode and resistors symbols, and the emitter arrow in the BJT. But otherwise, yeah, that Wilcox schematic is a fine example of the art.Part of the style, I think, is allowing yourself to reserve space just to have around the parts. Another part is the line width / weight, and white balance of the page. Which are difficult to do from electronic media because active-light raster displays (CRT, LCD, etc.) look and scale differently than printed paper.Tim

author: c4757p
author_rank: Super Contributor
timestamp: January 22, 2015, 05:10:49 am
content: Here's my usual style. This should be large enough to capture just about everything. Still a WIP, but not bad schematics

author: DIPLover
author_rank: Regular Contributor
timestamp: January 22, 2015, 05:36:20 am
content: Quote from: c4757p on January 22, 2015, 05:10:49 amI like your style, this is good!Why are some of your transistors in a semi-circle and others not?Also I think I found one more thing I like about the Wilcox drawing : the use of balls at the pins and asterisks in the name of active-low signals. It might be outmoded, but I think it looks way better, especially in busy bus structure where there is already densely packed horizontal lines. The bar over the net names makes for very noisy bus structures in comparison.

author: c4757p
author_rank: Super Contributor
timestamp: January 22, 2015, 05:41:36 am
content: Quote from: DIPLover on January 22, 2015, 05:36:20 amI use circles like that to indicate unconventional packaging arrangements - the semicircled transistors are matched pairs, kind of like how the series diode pairs are circled to indicate that they're together in the package. I omit the circles for single parts because I find they clutter the schematic.Quote from: DIPLover on January 22, 2015, 05:36:20 amI'm trying to decide whether or not I agree. So far I've been using an overline, but I see your point about a busy structure. Not sure whether I want to keep the overline, or use an asterisk like you said (WE*), or a dot - which is what it looks like to me in your scans - (WE•), or a hash (#WE).

author: MikeM100
author_rank: Newbie
timestamp: January 28, 2015, 05:58:18 pm
content: This topic has been a long time hobbyhorse of mine. I look at some circuit diagrams and just hate them !I would like to nominate 'Elektor' magazine (UK & Europe) for some of the 'nicest' circuit diagrams (schematics). I recently met one of their editors and he told me that they still use 'graphics' people to tidy up their diagrams.My pet hate is the modern trend for jumbles of components connected only by their net labels - no readability whatsoever.I recently saw a circuit with a (pullup) resistor plonked down on its own with two net labels - one to Vcc and one to an IC input !An interesting topic.

author: c4757p
author_rank: Super Contributor
timestamp: January 29, 2015, 04:13:01 am
content: Quote from: MikeM100 on January 28, 2015, 05:58:18 pmThis should be punishable by death.(okay, maybe notdeath...)

author: Mike Warren
author_rank: Unknown
timestamp: January 29, 2015, 05:13:02 am
content: Quote from: c4757p on January 29, 2015, 04:13:01 amI agree. Death is far too good for them.