The best schematic layout standards

[VK3DRB]

Hi all.

Some people get a little agro about schematic payout practices. For example, "NEVER use wires with net labels on them going nowhere - it is not a wiring diagram". There is no real reason for such an argument other than bad experiences or sheer pig headedness.

I think a paradigm reset is required. A fundamental requirement of a schematic is to effectively communicate how a circuit is assembled symbolically. Of course using it as a source to produce a subsequent PCB or a BOM is also fundamental. But if it does not communicate efficiently (shortest time to absorb the required information into the brain of the reader), it is a bad schematic.

In other words, for the same reader or the next person down the line a good schematic is one which is easy to  understanding. Many old TV schematics were examples of bad schematics - the good ones at least had sample waveforms on them and words depicting each functional subsection. (These days, you don't even get a schematic.)

I believe there are valid reasons to have open schematic wires with net labels to unclutter a schematic in certain instances, as there is to use bus lines and discrete wires. It all depends upon the situation, what the signals are, and the schematic environment.

Evenso we all have pet hates. Mine are:

- inconsistencies, especially in part and net labelling (cause: lack of planning or standards)
- no "NO ERC" markers on lines (cause: laziness)
- too many or not enough schematic sheets (cause: lack of planning)
- no history page or history information anywhere else (cause: laziness or poor standards)
- long symbolic component leads (eg: 20mm, rather than 10 or 15mm) (cause: using Altium's standard libraries)
- schematic layout that is hard to read or confusing (cause: not thinking of other readers)

To address these issues, I am developing PCB Coding Standards which are guideliness for developing PCBs. Such standards ensure we all read from the same page and no-one gets their noses out of joint. Also I am stating WHAT and WHY in the standards. I am purposely leaving many elements loose ended in that the designer has poetic licence to do how he sees it fit. But for component libraries, it is a THOU SHALL approach. I once worked for a medium size company where the libraries were and probably still are out of control, untrusted, full of errors and in multiple places.

Any comments, suggestions and war stories, on what you do for coding standards please add them here!

cheers,
Dave

[MacAttak]

My main thought is that I hope you keep in mind more than one schematic capture software package when you do this. Altium is in use by many professionals, but not by many hobbyists (and quite a few professionals too) due to the crazy price tag and reputation for being unstable. So it would be good to not assume that rule #1 of your schematic standards draft isn't "buy an Altium license".

[VK3DRB]

My main thought is that I hope you keep in mind more than one schematic capture software package when you do this. Altium is in use by many professionals, but not by many hobbyists (and quite a few professionals too) due to the crazy price tag and reputation for being unstable. So it would be good to not assume that rule #1 of your schematic standards draft isn't "buy an Altium license".

Agreed. I should have stated it was Altium centric. There are other schematic package around of course. As for stability, the latest Altium is greatly improved on earlier versions. One annoyance is bugs are not fixed unless you continue to pay. It is a bit like having to paying for a Windows upgrade from the Win ME to XP because of bugs. On the other hand, the number of users is limited and they need to have an income stream to stay viable and develop better products.

[AlfBaz]

- no "NO ERC" markers on lines (cause: laziness)

I don't like using these either but there are some common situations where disabling a certain ERC rule will prevent you picking up legitimate errors.
An example is an output pin feeding an input pin. You then place a series terminating resistor in line and you get a "no driving source" error for the input pin. With all the smarts altium has you'd think it would be clever enough to realise this.

To put my mind at ease I never place a "NO ERC" marker unless I have thoroughly investigated the error cause. If its a non-obvious error suppression I'll place a text footnote symbol or number near the "NO ERC" marker and expand on it in a text box else where on the schematic.

[Rufus]

Some people get a little agro about schematic payout practices. For example, "NEVER use wires with net labels on them going nowhere - it is not a wiring diagram". There is no real reason for such an argument other than bad experiences or sheer pig headedness.

Never say Never but stuff like the attached (Hello Dave?) really pisses me off. Is ADC-IOUT a helpful label allowing it to be referenced in other documentation? Perhaps it is a helpful identifier for the net in PCB layout?

Or perhaps it is a free pass to attach to that wire anywhere else in the schematic and the only way you can tell is to search the entire schematic for more instances of it.

edit addition:-
I once lifted some circuit from a Microchip evaluation board. Made PCBS and that bit didn't work. After some head scratching figuring out how that bit was supposed to work and why it wasn't I find a couple of pull up resistors attached by net labels sitting in the corner of the last page of their schematic. The cruddy CAD package they use for most of their stuff which produces PDFs with stroked font text which can't be searched doesn't help either.

I would definitely require net labels used to make connections to be placed on stubs and recommend that they be grouped and aligned to make finding other instances easier.

[AlfBaz]

Never say Never but stuff like the attached (Hello Dave?) really pisses me off. Is ADC-IOUT a helpful label allowing it to be referenced in other documentation? Perhaps it is a helpful identifier for the net in PCB layout?

Or perhaps it is a free pass to attach to that wire anywhere else in the schematic and the only way you can tell is to search the entire schematic for more instances of it.

I would definitely require net labels used to make connections to be placed on stubs and recommend that they be grouped and aligned to make finding other instances easier.

Unfortunately this can be an invaluable tool in identifying nets that require special attention in the PCB layout and this can always create arguments between those that use the schematic for circuit comprehension and those that use it to convey info to the PCB layout tools

[Neilm]

In other words, for the same reader or the next person down the line a good schematic is one which is easy to  understanding. Many old TV schematics were examples of bad schematics - the good ones at least had sample waveforms on them and words depicting each functional subsection. (These days, you don't even get a schematic.)

Where I work, you won't even get a schematic in the service manual. You get a block diagram  - although if I have written it any interesting signals will have a waveform if you need it to figure out if the board is faulty.

I believe there are valid reasons to have open schematic wires with net labels to unclutter a schematic in certain instances, as there is to use bus lines and discrete wires. It all depends upon the situation, what the signals are, and the schematic environment.

Evenso we all have pet hates. Mine are:

- inconsistencies, especially in part and net labelling (cause: lack of planning or standards)
- no "NO ERC" markers on lines (cause: laziness)
- too many or not enough schematic sheets (cause: lack of planning)
- no history page or history information anywhere else (cause: laziness or poor standards)
- long symbolic component leads (eg: 20mm, rather than 10 or 15mm) (cause: using Altium's standard libraries)
- schematic layout that is hard to read or confusing (cause: not thinking of other readers)

True - my pet hate is two wires joining in as they cross. I use Orcad and have had several problems when nets that should not connect when they cross have connected. I use new labels to try to avoid this.

I also don't like it when there are several nets run in parallel that snake of over the schematic but all head to different locations. You end up having to trace them out to work out where they go.

To address these issues, I am developing PCB Coding Standards which are guideliness for developing PCBs. Such standards ensure we all read from the same page and no-one gets their noses out of joint. Also I am stating WHAT and WHY in the standards. I am purposely leaving many elements loose ended in that the designer has poetic licence to do how he sees it fit. But for component libraries, it is a THOU SHALL approach. I once worked for a medium size company where the libraries were and probably still are out of control, untrusted, full of errors and in multiple places.

The libraries I use at work are fixed - if we don't use them then we don't get the information into the BOM. The worst problem is that they are maintained by the mechanical designers, so when they do a symbol I tend to have to ask them to alter it. Even if I have given them a note to say how I want the symbol to look.
Neil

[jmole]

Still learning altium, my main experience has been with EAGLE, but I think this is a decent rule:

Cross-sheet connections may only be through named ports, power nets, or ground nets.

[free_electron]

Still learning altium, my main experience has been with EAGLE, but I think this is a decent rule:

Cross-sheet connections may only be through named ports, power nets, or ground nets.

+1 on that !

[nctnico]

A few more rules for diagrams:
- no swastikas
- only T connections (no crossings)

[G7PSK]

Surely a circuit diagram should give enough information so that any one with a modicum of knowledge would be able to construct the circuit and it will work.
I have come across many diagrams that have been drawn on a cad program that do not allow this whereas the old diagrams that were drawn out by hand usually do, most likely due to the fact that the old school draughtsmen had experience in all fields of design and construction, I have come across this with other engineering drawings as well the cad operators had little or no practical experience during their training and so did not know how it works on the shop floor when making things.   

[Rufus]

Surely a circuit diagram should give enough information so that any one with a modicum of knowledge would be able to construct the circuit and it will work.

Not really. A part list and a net list provides the information required for someone to construct the circuit.

As the name implies a schematic should convey the scheme of the circuit. In most cases I would rather not see a schematic cluttered with detailed information required to construct it.

I think there is generally a conflict between designers who consider a schematic as something to represent and convey the scheme of a circuit and the CAD types who consider it to be a graphical entry method for producing net lists and part lists.

[c4757p]

As the name implies a schematic should convey the scheme of the circuit.

This is indeed what the name implies, but to me that's more of a block diagram. Those have their place as well, but I agree that a circuit diagram should convey all the necessary information that a reasonably knowledgeable engineer would need to build the circuit. Perhaps it's more that "schematic" is a poor name than that this is a poor method.

Obviously there are many "CAD types" who just vomit components and text onto a page and call that a schematic, but that doesn't mean reducing the amount of content is the right answer, it means it needs to be organized better.

[Rufus]

Obviously there are many "CAD types" who just vomit components and text onto a page and call that a schematic,

There are 'CAD types' who may insist schematics show component footprints or company database part numbers. Who may insist all schematic symbols show all power, no connect and mfg test pins. Who may insist schematics include symbols for mechanical items such as nuts and bolts and the bare PCB because they want a part list generated from the schematic to include them. Who may insist the schematic includes symbols for mounting holes (with no electrical connection) so a footprint for a mounting hold gets automatically pulled into PCB layout. Who may insist the schematic prominently includes "DO NOT SCALE" and "REMOVE ALL BURRS".

There is a whole host of crap 'CAD types' might want shown on a schematic which detracts from its primary function. Depending of course on what you think the primary function of a schematic is.

[nctnico]

Obviously there are many "CAD types" who just vomit components and text onto a page and call that a schematic, but that doesn't mean reducing the amount of content is the right answer, it means it needs to be organized better.

Time for an anecdote: one of the junior engineers in a company I worked for got the task of creating a rather large circuit consisting of several FPGAs and other stuff. Instead of creating several pages he created one huge diagram. When he printed it he spend quite some time taping the pages together. One of the senior engineers asked for wall-paper glue  We quickly gotten to the conclusion that the senior engineers should have given the junior engineer more support and we all goofed up.

[jmole]

There is a whole host of crap 'CAD types' might want shown on a schematic which detracts from its primary function. Depending of course on what you think the primary function of a schematic is.

Depends on what stage of the design process you're at. If you're building a board, the schematic you design for the board should definitely have stuff like mounting brackets, heatsinks, etc.

If you're at the conceptual stage, or SPICE simulation stage, probably there's no need for it.

This is why multi-sheet design is really great. Design subcircuits without the extra PCB mfg stuff, that you can run through SPICE, then use them as referenced documents in a larger sheet that is board specific.

[mikeselectricstuff]

I really hate what seems to be a recent trend of just dumping a load of symbols down, sticking some net names on and thinking that's Job Done.
OK for complex circuits, having wires drawn between all nodes can get complicated, but for simpler  ones it's just laziness, and makes it hard to read.
In particular it's very hard to see how many different places one net is connected to.

...I find a couple of pull up resistors attached by net labels sitting in the corner of the last page of their schematic

That is just unforgivable.

[AlfBaz]

Microchip are famous for this style of drawing and to top it off they publish the schematic as a non text searchable image, pasted into a PDF

[jmole]

In particular it's very hard to see how many different places one net is connected to.

One thing I like about EAGLE is the SHOW command, which will highlight all traces, pins, and PCB pads/traces with a given net name. Haven't found this in Altium yet, but I'm still exploring.

[AlfBaz]

One thing I like about EAGLE is the SHOW command, which will highlight all traces, pins, and PCB pads/traces with a given net name. Haven't found this in Altium yet, but I'm still exploring.

ALT + click on a net or line and CTRL + double click on a port to take you up a level

[mikeselectricstuff]

In particular it's very hard to see how many different places one net is connected to.

One thing I like about EAGLE is the SHOW command, which will highlight all traces, pins, and PCB pads/traces with a given net name. Haven't found this in Altium yet, but I'm still exploring.

That doesn't  help you if you're looking at a PDF

[grenert]

I really hate what seems to be a recent trend of just dumping a load of symbols down, sticking some net names on and thinking that's Job Done.

For years, this DIY audio company has been guilty of horrible schematics that make my head hurt:

[c4757p]

There are 'CAD types' who may insist schematics show component footprints or company database part numbers. Who may insist all schematic symbols show all power, no connect and mfg test pins. Who may insist schematics include symbols for mechanical items such as nuts and bolts and the bare PCB because they want a part list generated from the schematic to include them. Who may insist the schematic includes symbols for mounting holes (with no electrical connection) so a footprint for a mounting hold gets automatically pulled into PCB layout. Who may insist the schematic prominently includes "DO NOT SCALE" and "REMOVE ALL BURRS".

Why is this a bad thing, again? If the information is properly organized it won't get in the way. It's all part of the circuit design - why is some less important than others?

I really hate what seems to be a recent trend of just dumping a load of symbols down, sticking some net names on and thinking that's Job Done.

Yep. That is absolutely atrocious - there's no excuse for that. If I can't see at a glance if anything else connects to a certain point, you've failed.

[codeboy2k]

I really hate what seems to be a recent trend of just dumping a load of symbols down, sticking some net names on and thinking that's Job Done.

For years, this DIY audio company has been guilty of horrible schematics that make my head hurt:

That schematic has way too much audio magic for me
Lets see... LED  voltage references. check     ...  dual constant current sources.. check   ..  discrete opamp .. check!

thumbs up all around 

[Scutarius]

Hi everybody!

I was searching on google images the most eye pleasing schematics out there (tidy, organized, good practices, how to highlight info etc) just for having them on my desktop and taking a look for time to time.

Could you share in this post any of your personal sch that your are really proud of?

PS: I saw a post on LinkedIn about adding more information at the symbol level on passive components, I think it is worth it.
https://www.linkedin.com/feed/update/urn:li:activity:6707952060152844289/