Proper Schematics

[EPAIII]

While in another thread, I wrote this post on what rules schematic drawings should follow. This is not intended to be hard and fast. It is more like general guidance and sits on many years of work in electronics on my part OBSERVING the work of others. And it certainly is not the only way to produce a good schematic. But it does voice many of the principles that I have observed over those years. Virtually nothing here is/was an original idea on my part. OK, here it is:

First, what is a schematic? Or perhaps, what is NOT a schematic? Pictorial drawings with a representation of the physical appearance of the parts and with wires drawn to scale (big ones wider and small ones smaller) and in an expected appearance (rat's nest) when the parts are assembled is not a schematic. It may help beginners to identify the wires and where they go, but it does little or nothing to aid in understanding how the circuit works. This includes things like Fritzing. Then there are "hook-up" drawings which may show items as rectangular blocks and the wires between them, but little or nothing of what is in those parts. This may be needed, but it is not a schematic.

A schematic is a drawing of all the individual parts of a circuit. It is made with standard and easily understood symbols for those parts. And it shows all the wires or circuit paths between those parts. And it should be arranged to allow the viewer to UNDERSTAND the operation of the circuit with the least amount of effort on his or her part. That last part is very important and it distinguishes a good schematic from a rat's nest of parts and wiring that leaves the observer more confused instead of less. In short, a good schematic rapidly conveys HOW the circuit WORKS.

Drawing "proper" schematics is an art form, but with RULES. Yes, proper symbols are needed, as was brought out elsewhere. Nothing can be more confusing than a poor symbol. But there is much more.

Signal Flow:
The signal(s) should flow from LEFT to RIGHT and from TOP to BOTTOM. If possible, all inputs should be on the left and all outputs on the right. If they must be in the middle, then the same, LEFT to RIGHT convention should be followed: Text identifying the input and it's origin on the left, then the connector it comes in on, then the signal trace, and finally, at the right most point of this input circuit, the device it enters. Outputs that must be in the middle would be the reverse order, but the flow is still left to right.

I have seen schematics where the left to right was not wide enough, in spite of 24" or wider paper. So the signals were brought back to the left with long traces that also served to divide the top and bottom segments of the schematic. Those signal traces should not be crossed by other signals, if possible. Let them serve to divide the schematic in half. Then the left to right flow was continued on the bottom of the page. This made the overall circuit easier to understand.

Sometimes blocks are needed but they should be arranged left to right and top to bottom. Go with the flow!

Power:
Positive supply lines on top. Negative supply lines on bottom. Ground also on bottom or in middle if there is a negative supply. Actually draw the power busses instead of just sprinkling "+__" and "-__" and "Gnd" tags all over the place. Power also flows from left to right and top to bottom, just like signals. This becomes enormously more important when making large, complicated schematics with hundreds and hundreds of parts on one page. However, if you must use the tags, then follow the top and bottom rules.

Other rules?
Many modern components have a large number of connections. I like component blocks to have the +Voltages on top and the -Voltages and/or Ground on the bottom. That's it for top and bottom. Inputs on the left and outputs on the right. If a pin can't be classified as either an in or an out, then some judgement is needed. I suppose if it connects to +V it could be on the top. Or if to -V or Ground, then it could be on the bottom. The 555 timer has an external arrangement of Rs and C which is a good example of pins that should be on the left.

That's my two cents worth. Again, not carved in stone, but general guidance. I am sure there will be other opinions. And additional rules.

Let the games begin.

[Damperhead]

Totally agree!
I recommend checking out these documents before starting circuit diagram work or even considering it:

Overview of IEEE Standard 91-1984. Explanation of Logic Symbols:  https://www.ti.com/lit/ml/sdyz001a/sdyz001a.pdf
IEEE standard Symbols Appendix A: http://wakerly.org/DDPP/DDPP3_pdf/IEEEsyms.pdf
IEEE Std 315-1975. Graphic Symbols for Electrical and Electronics Diagrams (Including Reference Designation Letters): https://www.ee.iitb.ac.in/~spilab/Tips/ansii_graphic_symbols_for_electrical_and_electronics_daigrams_1993.pdf

These are old documents, but they provide valuable information on how the schematic symbols should be described. The implementation method with modern tools may be different, but the principle should be the same.


It is especially important that the circuit diagram editor is configured correctly, that line widths, fonts, links, reference designators, values, etc. are clearly visible after PDF export. Thus, circuit diagram documentation becomes more versatile, e.g. for maintenance, lab purposes, even for the customer. I know of many cases where the original circuit diagrams have had to be redrawn because they did not suit all stakeholders. They either contain too much sensitive information or no proper information at all.

[srb1954]

Good basic rules to follow.

Anyone who has developed commercial electronics eventually comes to realise that the function of the schematic is not just as input to the PCB CAD system but it should also be an easily human readable document to convey vital information to the factory and field technicians who build, maintain and troubleshoot the equipment.

However, a lot of people seem to forget or ignore this important role of the schematic drawing. I strongly dislike the current trend of drawing schematics where components are just thrown onto the schematic and not grouped together with their associated components. Nearly every pin on each component is then just labelled with a net name and one is left scrambling to find all the other components connected to that net. Highly frustrating and very error prone as you can't guarantee you have identified all the connections on a net. It is much better to apply much more thought to the initial layout so associated components are grouped together such that the flow of the connections between components is more local and can simply be directly drawn where ever possible.

The use of net names to interconnect disparate parts of the circuit should be minimised as far as possible and really only used for communicating between sheets in multi-sheet schematics. The off-sheet connections should be lined up on the edges of the sheet and it is really good practice to, as far as possible, line up the positions of the off-sheet connections with the sheet that they are traveling to. That way the multiple sheets can be pinned up on the wall and the flow of interconnected nets can be readily seen.

It can still be good practice to use some label nets even where they don't go off sheet as this can be a useful aid to explaining the circuit function. Net names should, as far as possible, describe the signal function clearly and concisely should be neither too long nor too abbreviated.

[EPAIII]

Great points. Keep them coming!

[Jwillis]

Another approach when doing highly complex designs is to use Hierarchical Schematics . Flat or single sheet schematics can become extremely confusing to use . So break up the design into smaller groups on separate sheets.  A couple articles on two different platforms you might consider looking at . https://embeddedcomputing.com/technology/analog-and-power/kicad-hierarchical-sheets-for-enhanced-schematics  and  https://resources.altium.com/p/flat-vs-hierarchical-schematics-why-you-need-dynamic-schematic-compilation#flat-vs-hierarchical-schematics-which-should-you-use

[807]

...Power also flows from left to right and top to bottom, just like signals...

Hmm...this is where I tend to draw my power lines differently. I have always had my power lines coming in from top right. Probably because when I started out in the 70's, I was mainly concerned with audio amplifiers & AM/FM transmitters.

With the output of the audio/RF amplifier on the right of the schematic, the raw voltage needed to power the output stage would also need to be on the right of the drawing. The lower powered pre-amp or vfo/signal generator parts using less current, and being on the left side of the schematic, would generally be decoupled or powered through a voltage regulator from the raw power supply.

The schematic would look awkward if the power supply came in from the left.

[807]

...I strongly dislike the current trend of drawing schematics where components are just thrown onto the schematic and not grouped together with their associated components. Nearly every pin on each component is then just labelled with a net name and one is left scrambling to find all the other components connected to that net. Highly frustrating and very error prone as you can't guarantee you have identified all the connections on a net. It is much better to apply much more thought to the initial layout so associated components are grouped together such that the flow of the connections between components is more local and can simply be directly drawn where ever possible...

I agree. Only yesterday, I saw this simple AM transmitter circuit with unneccesary net names. There was no need to draw it this way. It just takes longer to work out the circuit. It's such a simple circuit that the "MOD", "Drive" & VCC net only needed to have a line drawn between them.

...and even then, it still breaks some of the "rules".

https://content.instructables.com/FHU/LS4B/LCBYFG8T/FHULS4BLCBYFG8T.png?auto=webp&frame=1&width=1024&height=1024&fit=bounds

[barshatriplee]

Here is a very good write-up on how to check schematics:

https://welldoneblog.fedevel.com/2013/11/25/8-step-schematic-checking-procedure/

It is very important to check schematics. Otherwise, there may exist many small and big mistakes. No checking can lead to a malfunctioning circuit. It is very important to check before printing the PCB.
PCB inspection is also very important in the device manufacturing process. Here is also a write-up about the basics of PCB inspection:

https://www.pcbway.com/blog/Engineering_Technical/3_Basics_Of_PCB_Inspection.html

[TimFox]

My contributions, as one retired after 40 years:
1. Power busses indicated by arrows to +5V, etc. can help by uncluttering the schematic.  Done carefully, they are no worse than ground symbols.
2. A somewhat controversial rule, which I follow rigorously, is that when wires cross, there is a "hiccup" but no connection.  Connected wires should be offset (vertically or horizontally) so that they form Tees, not Crosses, with a connection dot.  This never causes a real problem, and avoids confusion between the two cases (connect or no-connect).
3.  My work is almost all analog, but in a digital circuit with a 16-bit parallel output connected to a 16-bit parallel input, drawing this locally with the usual bus notation and node names can unclutter the schematic.
4.  When signals need to leave the page to another page, the symbol should include the destination page number as well as the node name.

[m k]

Destinations with rows and columns of bigger sheets are also positive.

Dotted or not has never been a problem here, same with US symbols or not.
Maybe because of frequent variations and so none dominating.

[artag]

However, a lot of people seem to forget or ignore this important role of the schematic drawing. I strongly dislike the current trend of drawing schematics where components are just thrown onto the schematic and not grouped together with their associated components. Nearly every pin on each component is then just labelled with a net name and one is left scrambling to find all the other components connected to that net. Highly frustrating and very error prone as

Exactly. And it has a severe problem : whilst it may be possible to find the matching netname, there is no way to tell if it's the _only_ matching netname - it may go to several destinations.

These are not schematics. They're just a very ineffficient way to enter netlists.  If that's all you want to do, enter them directly and perhaps alphanumerically - try to get at least some advantage out of your laziness.

 

[Benta]

I agree. Only yesterday, I saw this simple AM transmitter circuit with unneccesary net names. There was no need to draw it this way. It just takes longer to work out the circuit. It's such a simple circuit that the "MOD", "Drive" & VCC net only needed to have a line drawn between them.

...and even then, it still breaks some of the "rules".

https://content.instructables.com/FHU/LS4B/LCBYFG8T/FHULS4BLCBYFG8T.png?auto=webp&frame=1&width=1024&height=1024&fit=bounds

A nice example of how NOT to do it. But it's incomplete. The real die-hards place a dotted-line rectangle around each "block" to demonstrate their "modular" and "object-oriented" thinking.

[schmitt trigger]

We hold the following statements SHOULD be self-evident. But they are many times ignored.

Drawing a schematic is like drawing a city map: it allows a person unfamiliar with it to navigate it.

The better maps have lots of additional information: locations of subway stations, points of interest, location of geographic features, names of bridges, etc.

A schematic functions exactly the same. Thus the best way to determine whether the schematic is any good, is to give a board and schematic to someone who isn’t familiar with it, and see how long it takes him to trace a signal.

[m k]

Automation schematics are many times few kilos of paper.
There stuff per page and their placings are quite important.
Coming from electronics is a bit of a burden since good automation pages are using all positions of the page and wiring is many times minimal.

Now when schematics drawing software is a norm but cheap ones are lacking functions we are clearly seeing how these two schematics types are closing.
For example it's obviously trivial to rearrange 10 automation schematics pages as you will, after copying double sides to single sides.
But if schematics drawing software is not supporting block move with wiring the user will easily drop wiring and start using this limited information block style.

[tggzzz]

I'll emphasis other peoples' support for:

• design patterns. There are certain standard easily recognisable ways to draw subcircuits, e.g. an op-amp integrator, a current source, a filter. Use them.
• wires, not netlist names. Where helpful, use busses with names wires at entry/exit points. Exception: power supplies. Netlist names might work in the CAD package, but fail on paper and in PDFs with multiple pages/schematics.
• hierarchical schematics. Multiple schematics at one level are equivalent to software where all variables and functions are global
• left to right and top to bottom signal flow. Exception: feedback paths. I wonder if the right-to-left schematics are due to laziness/ignorance, or the artist is from a country where writing is from right to left?

[AndyC_772]

There's definitely room for some personal taste and preference here.

I'm not a huge fan of wires that stretch a long way across a schematic, especially if there's a bunch of them all together so the eye can easily lose track of which is which. If the schematic looks like one of those mazes that are printed on the place mats at 'family friendly' restaurants, then it's only making life difficult for the reader. Nobody should have to go over a schematic using different coloured highlighter pens just to trace where the individual wires in a bundle actually end up.

As for hierarchy: yes, iff there are parts of your design that have multiple, identical instances, in which case of course it makes sense to draw the schematic once and instantiate it multiple times.

Otherwise, it's important to recognise that 'forced' hierarchy means following signals around the design not only takes longer, but it also introduces the possibility of errors. For example, I once inherited a design which had been divided up this way, and a net name at the bottom level ended up attached to a port with a different name, that had another different name again at the top level, before getting a new different name yet again at a different lower level. Unravelling that mess to figure out what was connected to what took ages, and the hierarchy added absolutely nothing useful.

IMHO a net with a name on one page should be connected to an identically named net on another. (Think: suppose you have a printout of the schematic with those two pages side by side on your desk; how can you tell by looking that they are not connected together, if in fact each has a 'local' scope by virtue of hierarchy).

[TimFox]

I'll emphasis other peoples' support for:

• design patterns. There are certain standard easily recognisable ways to draw subcircuits, e.g. an op-amp integrator, a current source, a filter. Use them.
• wires, not netlist names. Where helpful, use busses with names wires at entry/exit points. Exception: power supplies. Netlist names might work in the CAD package, but fail on paper and in PDFs with multiple pages/schematics.
• hierarchical schematics. Multiple schematics at one level are equivalent to software where all variables and functions are global
• left to right and top to bottom signal flow. Exception: feedback paths. I wonder if the right-to-left schematics are due to laziness/ignorance, or the artist is from a country where writing is from right to left?

-hp- and other manufacturers used to highlight feedback paths with heavy dashes or other highlights to distinguish them from "forward" signal paths.

[tggzzz]

There's definitely room for some personal taste and preference here.

I'm not a huge fan of wires that stretch a long way across a schematic, especially if there's a bunch of them all together so the eye can easily lose track of which is which. If the schematic looks like one of those mazes that are printed on the place mats at 'family friendly' restaurants, then it's only making life difficult for the reader. Nobody should have to go over a schematic using different coloured highlighter pens just to trace where the individual wires in a bundle actually end up.

Counterexample, from the Tek 485.

There are a number of 15V tant bead capacitors on a 13V line (oops!). It is a right royal pig to find them all because the the 13V line "tunnels" all over several schematics. Yes, I had to use highlighter to discount the irrelevant and to find the relevant little buggers.

But if it is a bundle of related wires, then use a schematic's bus notation. Obviously that works for address and data busses, but it is also completely satisfactory for control signals (e.g. CS, RW) as well.

As for hierarchy: yes, iff there are parts of your design that have multiple, identical instances, in which case of course it makes sense to draw the schematic once and instantiate it multiple times.

Otherwise, it's important to recognise that 'forced' hierarchy means following signals around the design not only takes longer, but it also introduces the possibility of errors. For example, I once inherited a design which had been divided up this way, and a net name at the bottom level ended up attached to a port with a different name, that had another different name again at the top level, before getting a new different name yet again at a different lower level. Unravelling that mess to figure out what was connected to what took ages, and the hierarchy added absolutely nothing useful.

I disagree, for two necessary reasons.

If there are multiple instantiations of lower level schematics then there must be some different naming at different levels. For example each instantiation of the subcircuit would have a "CircuitSelect" wire connected to a "pin/connector", but the higher level schematic would have one CircuitSelect1...CircuitSelectN wire connected to each instantiation's "pin/connector".

By way of analogy, would you insist in a computer program that the argument names in a procedure definition are the same as the variable names where the procedure is invoked? For example, if someone else implemented a function
double sin(double angle){...}
would you prefer my code to be
angle=alpha;
foo=sin(angle);
angle=beta;
baz=sin(angle);

or more simply

foo=sin(alpha);
baz=sin(beta);

IMHO a net with a name on one page should be connected to an identically named net on another. (Think: suppose you have a printout of the schematic with those two pages side by side on your desk; how can you tell by looking that they are not connected together, if in fact each has a 'local' scope by virtue of hierarchy).

Yes, where ever possible - but not where that cannot be possible

But, as ever, good taste is important in art.

[T3sl4co1l]

I wrote this a long time ago... which, could probably use some updating, but isn't very relevant anymore, anyway:
https://www.seventransistorlabs.com/tmoranwms/Elec_Circuit_Rules.html
I mean, the placement rules are fine I guess.

Neat fact: there weren't any good free schematic tools at the time.  Falstad was around but is pretty marginal for printing purposes.  KiCAD I think was still very basic at the time (and the less said about gEDA the better?).  There was a number of SPICE tools of course, all of them with ugly symbols.  So, you were as well off copying and pasting from existing schematics... which never matched.  So, I took it upon myself to draw my own, roughly at 100 DPI.  I also started on some 300 DPI symbols, but didn't get much use out of them by the time available tools improved (and I eventually picked up Altium for real).

Nowadays, CircuitLab is free online and looks good, and KiCAD is free and usable (and some libraries look alright), so there's very little reason to paste images and draw pixel by pixel.

As for higher level rules, nowadays I insist on three-way junctions, aligning components to make sensible rows and columns, and distributing space so that labels are clear and associated with their part (occasionally hiding labels only when identical components are grouped together).  The simplest way to describe it is layout akin to the \$\LaTeX\$ engine, where spacing and positioning is adjusted based on constraints and a heuristic. It's done by hand of course, but that's the sort of principle I apply.  Not that this means anything to those who don't know \$\LaTeX\$ algorithms; reading up on it is suggested reading at least, it's good to know for optimizing / dynamic programming approaches.

And for larger schematics, I use a mix of hierarchical and multi-sheet approaches.  When subcircuits are one-off, hierarchy doesn't offer much value, but occasionally there's value in showing the connectivity.  When subcircuits are repeated, hierarchy is nearly mandatory.

Tim

[tggzzz]

I wrote this a long time ago... which, could probably use some updating, but isn't very relevant anymore, anyway:
https://www.seventransistorlabs.com/tmoranwms/Elec_Circuit_Rules.html
I mean, the placement rules are fine I guess.

You mention one interesting case where left to right and top to bottom should be broken, IMHO.

In the Tektronix Y-deflection circuits from the 4x5 era, the primary signal chain is through a succession of *Barrie Gilbert multiplier" circuits, e.g.


There the natural signal flow within a subcircuit is from bottom to top. In some schematics that is very visible, in others it is concealed by omitting the transistors and just drawing the ICs with the signal entering on the left and leaving on the right.I

Design patterns are there to be broken (but only when dictated by good taste!).