How to design pretty schematics? Style guides? Tutorials? Examples? Software

[timofonic]

hello.

I would like to draw good looking and easily understandable schematics, I just try to make them the smallest possible because some OCD shit but I'm unable to make them good looking.

I also dislike the style of most EDA software, they look ugly and difficult to understand if being complex. I dislike Eagle and DipTrace styles, for example.

I like the style of this software: sPlan

Can we update this topic? Or maybe I missed something else.

Best regards.

[Vipu]

http://ecee.colorado.edu/~mcclurel/schematic_best_practices.pdf

[timofonic]

http://ecee.colorado.edu/~mcclurel/schematic_best_practices.pdf

Thanks! I did look at them, it seems interesting. If it includes schematic examples of correct vs wrong, it would be perfect. Sometimes visual information makes me to remember it better.

I draw things this way. Strong OCD.

 I find the frame design to be very interesting, specially the memo part. It can save an extra page.

What software do you use?

What's that common obsession to use yellow on ICs? I find it eye-bleeding! I know it's common in EDA software.

It's not bad at all. I'll publish some of my awful designs, they are very simple schematics.

Best regards

[free_electron]

I draw things this way. Strong OCD.

AAAAAGH . MY EYES !!!!

[T3sl4co1l]

Style guide?

This is generally applicable: http://seventransistorlabs.com/tmoranwms/Elec_Circuit_Rules.html

If you've studied typography or typesetting at all, you've probably heard of LaTeX; the algorithms perform a (usually heuristic) minimization of "badness" (as it is called), usually extending to the paragraph level: inter-letter and inter-word spacing are varied to get the correct line wraps (hyphenating the break if necessary).  The process is repeated for lines and paragraphs on a page, and "floats" (figures and tables) are placed and the text flowed around them.  Built-in table functionality kind of stinks, but the most recent packages for table formatting are pretty great, bringing much of the space-adjusting, badness-minimizing power to bear upon paragraphs within cells, and between the width and height of cells (and page wraps if necessary and allowed).

If you think of formatting a schematic in the same light, you'll come to see that every component has a certain "personal space", occupied by the symbol itself, its labels, and a certain amount of necessary white space which visually distinguishes and separates it from its neighbors.  The labels take up space and necessarily modify that bubble.

Wires must be routed between components according to the netlist, but similar constraints can be placed: especially if net labels are used, they should be spaced out so the labels are not ambiguous; straight lines are preferred, with a horizontal bias for signals, and a vertical bias for power/ground branches.  Signal flow should be from left to right if possible, just as English reading order is left to right; and each signal path should be its own line, just as English text should be in easily readable lines.

http://seventransistorlabs.com/Images/LED_Light.png
Here's an example of a circuit which is broken into multiple 'lines', even despite some parts being apparently reversed (note the fan startup circuit takes wires that cross over, to allow the correct left-to-right signal ordering).  The horizontal bias with vertical power/ground branches is particularly strong on the bottom line, with bias/sense resistors making several vertical branches between the horizontal signal or supply rails.

Tim

[BlueBill]

I've been using an antiquated version of OrCAD 10.3 for ages. I never had the need to update it and got comfortable with the workflow.

I use Sprint Layout for PCB work. Again, I like the workflow.

[KM4FER]

A personal opinion on style:

I hate schematics where resistors are drawn as rectangles instead of zig-zag lines.   
In fact if I see one drawn this way I will often move on to something else unless I am really, really interested in it and then I will curse the whole time I am studying it.

My reasoning is that there are so many circuits these days that have IC's in them, which are drawn as rectangles, that if resistors are drawn as rectangles as well it is not obvious if the component is an IC or a resistor unless you take time to read the labels or count terminals.  A good schematic should allow an experienced observer to quickly get an overview of the circuit in a quick glance.  As an example suppose you have an IC with pull-up resistors on several pins.  With zig-zags it is easy to see at a glance that they are resistors and then to determine that they are pull-ups.  With rectangles one has to stop and look closer to see that the component is a resistor and not another IC and then conclude that it is a pull-up.

For more than 100 years resistors have been drawn as zig-zags.  It is only fairly recently when rectangles seem to have come into vogue.  Where did this ever come from anyway?  I'm guessing it all started when crude computer programs began to be used for drawing schematics and it was a lot easier/quicker to just draw a rectangle.  What's next:  capacitors as boxes, inductors as boxes?  Will everything become a box?

Come on people, think outside the box !

Rant over...
earl...

[free_electron]

A personal opinion on style:

I hate schematics where resistors are drawn as rectangles instead of zig-zag lines.   
In fact if I see one drawn this way I will often move on to something else unless I am really, really interested in it and then I will curse the whole time I am studying it.

My reasoning is that there are so many circuits these days that have IC's in them, which are drawn as rectangles, that if resistors are drawn as rectangles as well it is not obvious if the component is an IC or a resistor unless you take time to read the labels or count terminals.  A good schematic should allow an experienced observer to quickly get an overview of the circuit in a quick glance.  As an example suppose you have an IC with pull-up resistors on several pins.  With zig-zags it is easy to see at a glance that they are resistors and then to determine that they are pull-ups.  With rectangles one has to stop and look closer to see that the component is a resistor and not another IC and then conclude that it is a pull-up.

For more than 100 years resistors have been drawn as zig-zags.  It is only fairly recently when rectangles seem to have come into vogue.  Where did this ever come from anyway?  I'm guessing it all started when crude computer programs began to be used for drawing schematics and it was a lot easier/quicker to just draw a rectangle.  What's next:  capacitors as boxes, inductors as boxes?  Will everything become a box?

Come on people, think outside the box !

Rant over...
earl...

IEC norm has a resistor as a box.
IEEE has it as wavy line

pick your norm

[Rufus]

I hate schematics where resistors are drawn as rectangles instead of zig-zag lines.   
In fact if I see one drawn this way I will often move on to something else unless I am really, really interested in it and then I will curse the whole time I am studying it.

Wow, really ignorant yank...

Try looking up IEC 60617 or the British, German, and Australian standards that proceed it.

[tggzzz]

Personally I'm easily satisfied. All one has to do is:

• have signals flowing from left to right and top to bottom; not right to left, not bottom to top
• connect all relevant pins together with black line; don't draw a small wire next to each pin, label it frozbat123, and let the reader guess whether they have seen all the pins connected to wire frozbat123
• "standard" subcircuits (e.g. inverting opamp, common-collector amplifier) will have components placed in a "standard" pattern; follow the pattern so that readers can quickly spot what they don't have to understand in detail.
• have +ve rails at the top, gnd in the middle and -ve at the bottom

Far too many diagrams don't seem to follow that minimal amount of "goodness"

[KM4FER]

OK,  Yes I will admit that I am an ignorant Yank.  That's one reason I like EEVBlog so much.  Since I can't travel there I am getting to see how the rest of the world thinks.

earl...

[zeke]

I am betting that someone is going to ask the same question about designing pcb layouts.

So here is the link to Dave's PCB Design Tutorial.

[SL4P]

Personally I'm easily satisfied. All one has to do is:

• have signals flowing from left to right and top to bottom; not right to left, not bottom to top
• connect all relevant pins together with black line; don't draw a small wire next to each pin, label it frozbat123, and let the reader guess whether they have seen all the pins connected to wire frozbat123
• "standard" subcircuits (e.g. inverting opamp, common-collector amplifier) will have components placed in a "standard" pattern; follow the pattern so that readers can quickly spot what they don't have to understand in detail.
• have +ve rails at the top, gnd in the middle and -ve at the bottom

Far too many diagrams don't seem to follow that minimal amount of "goodness"

I love you ! 

[tggzzz]

I love you ! 

Fortunately we are literally a world apart

[c4757p]

My reasoning is that there are so many circuits these days that have IC's in them, which are drawn as rectangles, that if resistors are drawn as rectangles as well it is not obvious if the component is an IC or a resistor unless you take time to read the labels or count terminals.  A good schematic should allow an experienced observer to quickly get an overview of the circuit in a quick glance.  As an example suppose you have an IC with pull-up resistors on several pins.  With zig-zags it is easy to see at a glance that they are resistors and then to determine that they are pull-ups.  With rectangles one has to stop and look closer to see that the component is a resistor and not another IC and then conclude that it is a pull-up.

Resistors have a much longer aspect ratio than ICs, are much smaller, have only two pins, and don't have labels inside. If you can't recognize them quickly, perhaps you should have your eyes checked?

[kizzap]

Resistors have a much longer aspect ratio than ICs, are much smaller, have only two pins, and don't have labels inside. If you can't recognize them quickly, perhaps you should have your eyes checked?

I personally prefer the European method, with boxes for resistors, as the OCD in me finds it easier to draw a box, then get the squiggly line right. The only problem I have with it is that the symbol for an inductor seems to also a box, albiet solid.

[T3sl4co1l]

I use very specific proportions on my resistor squiggles, perhaps that would help?

Typography is just OCD with [usually] imaginary bounding boxes.  If you can see those, you can OCD all you like, *and* get a useful and nice schematic.

Tim

[AndyC_772]

I have a few other design rules which I've found helpful:

When designing symbols for ICs, I normally separate them out into signal pins and power pins, on two different parts of the symbol. The power symbols and the associated decouplers are kept on another page, so the signal flow isn't cluttered with power pins and capacitors.

Every IC has every pin shown on the symbol, always. No hidden pins, for any reason, ever. No bus pins either.

Power supply rails are always labelled with their actual voltage, and never 'VCC' or similar. A net called +3V3 is unambiguous, but a net called VCC could be 5V, or 3.3V, or 1.25V, or anything else. Using the specific voltage reduces the chance of accidentally connecting dissimiliar supply rails together. (Exception: supply rails whose voltage is not fixed may be called by something else provided it's unambiguous, eg. VDD_CORE).

The addition of helpful comments about how the design works, and why specific components or circuits are used, IS permitted!

The use of hierarchy is generally NOT encouraged, unless there are multiple, identical instances of a specific block. It's much easier to follow a signal from page A to page B than it is to follow it from page A, up a level to page 0, and then back down to page B where it appears under a slightly different name. If you need a block diagram, then draw a block diagram... don't try and force the schematic into a structure that gives you one "for free".

Where hierarchy is used, each signal must have exactly one identical, unique name across the whole schematic. So, for example, a signal called CPU_CLK on one page mustn't end up getting called CLK_CPU or CPUCLK_33M elsewhere.

[Warhawk]

At work, We use this marking for power nets:

P3V3 - 3.3 V
1P3V3 - 3.3 V second rail
2P3V3 - 3.3 V third rail...

V is decimal point
P means positive
N means negative e.g. 1N3V3 is second rail -3.3V

Then we use M for common ground (I think it comes from German "Masse"). M, 1M, 2M etc.

I like it and use it for my personal projects as well.
 

[daqq]

I can't give you a how to, but there are several things that I honestly HATE and I have seen on too many occasions:

Physical instead of logical - some people draw the schematic symbol for parts to match the actual layout on the part - this is OK-ish for small parts (555), but when you see a 128 pin square with pins and nets coming out of all sides, rotated willy nilly, a crystal crammed sligthly sideways onto the schematic and see that it is a microcontroller, that's just nasty. Yes, it might save some time while drawing the part schematic symbol, but other than that it's pretty much useless. Example: http://designer.mech.yzu.edu.tw/articlesystem/article/compressedfile/%282006-09-01%29%20Chapter%203%20%20Design%20of%20the%20Distributed%20Data%20Server.files/image003.jpg (I've seen worse though)

Ignorance and avoiding of hierarchical design. Use at least some level of block design (separate schematic pages for block and such) - while you CAN jam a relatively big system onto one page, you really should not. I'd much rather see a half empty schematic page then a schematic page packed to the full with two grid units separating blocks.

Nets with no apparent purpose deducible from their name (such as "B4"). When you name stuff, you better mean it.

Connect with names rather than wires when dealing with more than a few wires. See: http://www.schmalzhaus.com/UBW/Images/44PinSchematic.png

[T3sl4co1l]

Physical instead of logical - some people draw the schematic symbol for parts to match the actual layout on the part - this is OK-ish for small parts (555), but when you see a 128 pin square with pins and nets coming out of all sides, rotated willy nilly, a crystal crammed sligthly sideways onto the schematic and see that it is a microcontroller, that's just nasty. Yes, it might save some time while drawing the part schematic symbol, but other than that it's pretty much useless. Example: http://designer.mech.yzu.edu.tw/articlesystem/article/compressedfile/%282006-09-01%29%20Chapter%203%20%20Design%20of%20the%20Distributed%20Data%20Server.files/image003.jpg (I've seen worse though)

And they're all logic active-low, even the VDD pin!

Nets with no apparent purpose deducible from their name (such as "B4"). When you name stuff, you better mean it.

Connect with names rather than wires when dealing with more than a few wires. See: http://www.schmalzhaus.com/UBW/Images/44PinSchematic.png

This one feels marginal to me.  I'd tolerate it.  It's at least as nice as possible given the style -- a good matrix fanout approach.  It does necessitate putting the crystal WAY >> OVER >> THERE though, which looks bad.  It's not obvious if a bus routing style would work here; if the nets were named, that might be more obvious!  Which, of course, includes the previous point: purposeful names, instead of generic or auto-generated names.  Only if they truly are general purpose buses (rare these days, outside of serial buses) should general names be used ("DB0", etc.?).

Using off-sheet connectors or labels to link the "floating" connectors would be the cleanest way, though.

Tim

[128er]

Physical instead of logical - some people draw the schematic symbol for parts to match the actual layout on the part - this is OK-ish for small parts (555), but when you see a 128 pin square with pins and nets coming out of all sides, rotated willy nilly, a crystal crammed sligthly sideways onto the schematic and see that it is a microcontroller, that's just nasty. Yes, it might save some time while drawing the part schematic symbol, but other than that it's pretty much useless. Example: http://designer.mech.yzu.edu.tw/articlesystem/article/compressedfile/%282006-09-01%29%20Chapter%203%20%20Design%20of%20the%20Distributed%20Data%20Server.files/image003.jpg (I've seen worse though)

Looks like a schematic from a AVR application note I've seen yesterday. Except for the "all active-low pins". It's probably a feature, not a bug 

http://www.atmel.com/images/atmel-2521-avr-hardware-design-considerations_applicationnote_avr042.pdf

Is this type of symbol maybe from a Altium standard library?

Edit: The schematic is on page 14

[T3sl4co1l]

For showing the device and pinout, that's not unreasonable; the port pin types appear to be bidirectional, which is consistent.  If it's in their library for actual schematic use, it would be annoying, though.

Tim

[Richard Crowley]

I personally prefer the European method, with boxes for resistors, as the OCD in me finds it easier to draw a box, then get the squiggly line right. The only problem I have with it is that the symbol for an inductor seems to also a box, albiet solid.

Or a fuse or any of the other seeming half-dozen or so components that are all shown as a generic rectangle.
And left to the reader to sort it out. I don't like it. It violates Al Einstein's rule of oversimplifying things.
The one thing it has going for it is that you can place text (like the reference and/or the value) INSIDE the box.

[daqq]

Nets with no apparent purpose deducible from their name (such as "B4"). When you name stuff, you better mean it.

Connect with names rather than wires when dealing with more than a few wires. See: http://www.schmalzhaus.com/UBW/Images/44PinSchematic.png

This one feels marginal to me.  I'd tolerate it.  It's at least as nice as possible given the style -- a good matrix fanout approach.  It does necessitate putting the crystal WAY >> OVER >> THERE though, which looks bad.  It's not obvious if a bus routing style would work here; if the nets were named, that might be more obvious!  Which, of course, includes the previous point: purposeful names, instead of generic or auto-generated names.  Only if they truly are general purpose buses (rare these days, outside of serial buses) should general names be used ("DB0", etc.?).

Using off-sheet connectors or labels to link the "floating" connectors would be the cleanest way, though.

Tim

Well, most of the stuff in the thread is meant as rule of thumb. You are right, it's better to connect stuff like crystals and small miscellany directly, I was talking more along the lines of SPI connections or higher.