Im going to guess the answer is yes, many many better ways to do it…but here is what I have!
I’m trying to recreate what I have going on here, but in schismatic form, as frankly what I have I think is right, but boy is it ugly!
Actually the only thing which may be deemed lacking in your schematic is an indication that the switch has a center off position. Otherwise I do not see anything wrong with it…it is clear enough.
One thing I try to avoid is unneeded wire crossings. But if you want your schematic to show pins 1,3,4,6 in that order then I do not see any good way around that.
An alternative draw could rotate the two capacitors on the right each by 90 degrees and place one further to the right than the other. I am not sure that the result would end up better.
Do you really have 5 nF capacitors or are they actually 4.7 nF? 4.7 is a standard E12 (I think it is 12?) value but 5.0 is not. Not to worry about that unless you have 5% or better tolerance on them (the acceptable actual value ranges overlap even with 5% tolerance.)
1 Like
Actually the only thing which may be deemed lacking in your schematic is an indication that the switch has a center off position. Otherwise I do not see anything wrong with it…it is clear enough.
Thank you, I’m here to learn anything that may, could and should be deemed lacking! So thank you. This was the first DPDT switch I found in the component .lib very new to this so to be 100% honest not sure what one with an off position would look like?
One thing I try to avoid is unneeded wire crossings.
Yes, this is the part that is worrying me as a bad habit, and was wondering if I should use netlabels instead?
But if you want your schematic to show pins 1,3,4,6 in that order then I do not see any good way around that.
Working my way through some tutorials, but have not got confident enough to edit a component and change the order without the fear of messing up and finding out I changed the wrong thing.
An alternative draw could rotate the two capacitors on the right each by 90 degrees and place one further to the right than the other. I am not sure that the result would end up better.
Thank you I will try that!
Do you really have 5 nF capacitors or are they actually 4.7 nF?
I actually do! I mainly work with vintage audio electronics, so have a lot of the old pre-modern standards, so lots of caps with values like 5nF, 25nf, 50uF and things like that…only now getting into the 21 century and moving form point to point wiring to PCBs 
Hello
I don’t see how this ca be changed. I think this is perfect and the crisscrossing of wires cannot be changed or even improved any further.
Although am trying to work on on this from my end and I will update you later on I don’t see any more serious changes coming in.
1 Like
I think you are doing OK. I usually like to show ICs (for example) in pin order but there are a lot of variations according to personal preference. The main thing about a schematic is that it should be clear and accurate. Also most of us prefer to have the input toward the left and the output toward the right. I think you are conforming to that convention.
1 Like
Netlabels , I detest schematics where basically almost each component has a net label rather then a connecting wire. You get these disjointed abominations of a diagram. It seems to infect Eagle users.
I group logical components together , micro and it’s support passives etc. I always show decoupling where it should be physically. Then I run net labels to the next block ( or sheet ). So for example the power regulator and associated components will be grouped and connected by wires etc.
If my Microcontroller drives an error led from an IO pin , it’s shown connected to that pin by a wire
A small number of crossing unconnected wires are fine as long as the function is clear.
2 Likes
A few weeks ago someone posted a great comment about that. I think they called such a drawing something like a “graphical netlist” instead of a schematic diagram. It was an excellent point. Too many net labels (instead of wires) make a schematic very difficult to read.
3 Likes
You can make this switch symbol organised the same way as real switch is - two rows of 3 pins and contacts shifted along them. Then you will be able to make this schematic without any crossing wire. But your schematic is clear enough to not spend a time on doing new symbol.
2 Likes
I try to adhere to “signals from left to right” and voltages from top to bottom.
Therefore I usually prefer to to set the capacitors upright.
It also makes it more clear that one of the switches goes to each of the capacitors, and the other switch goes to the other side of each capacitor.
It also sorts out the capacitors, At the moment pin 4 of the switch is going t the left of C7, while pin 6 is going to the right of the other C7.
I’m OK with crossing wires Drawing wires through text though is never a good thing, and rotating text is also seldom a good choice.
Changing font size also makes it look “Messy”.
Just use the same font for the same sort of thing.
Then, if you want to emphasize some detail, you can use bigger text or bold.
The small text is also probably more of a hindrance then a help. It just encouages zooming diseaze.
Just use more “paper” area. Trying to cram an ever growing schematic onto a single A4 sheet is a huge time waster. Over time it can very easily add up to multiple hours just rearranging stuff and drawing fancy lines. Those lines are also not clear. A bit of whitespace between schematic sections is a very clear indicator to separate sections. Don’t remove the whitespace by cramming stuff together.
The example below has become a big mess because lack of whitespace between the sections.
2 Likes
You could make it more symmetric by crossing the 2 wires at 45°, and/or turning the 2 C?s so that they are also graphically parallel to C10 (since they are also electrically).
1 Like
Thank you all for the excellent advice, and help.
Regards netlabels, and understandable disdain for their overuse making it hard for anyone else to read (love the term “graphical netlist”).
I’m starting to realise that with all the capacitor switches I have in the circuit its going to be more practical making 2 PCBs, one for the main circuit and one for all the toggle switches/caps.
Would this be an appropriate way to use netlabels?
(Really hope you don’t see this as me just ignoring all the solid advice, rather, just trying to adjust to the new two board idea)
1 Like
Yes that’s a nice compromise.
1 Like
That’s not too bad.
But having the same switch configuration nine times in the schematic, an idea could be to create a custom symbol for the switches and caps.
That would really clean up the schematic and make it very readable. Shape is not important, perhaps a box with a cap symbol and value 5/10/15 nF.
Just an idea.
1 Like
Thank you very much, your input in this thread has been really helpful, and very much appreciated!
But having the same switch configuration nine times in the schematic, an idea could be to create a custom symbol for the switches and caps.
That would really clean up the schematic and make it very readable. Shape is not important, perhaps a box with a cap symbol and value 5/10/15 nF.
Thank you, that’s a really good idea, as I’m going to have to make a footprint anyway for the switch, so makes sense to make a simplified symbol too so I have my own part ready to go when I want to use this same configuration in other projects.
With a custom symbol you could also split the switch into ±90° turned top and bottom parts with signals coming from top and bottom, mechanically connected with a dashed line in the shape of ], so that all 3 Cs are in the usual parallel circuit (like piggybacked or a backpack for C10).
Depends on what you want to express (whether someone first should see the common pattern of adding values to a capacitor, that a capacitance can change its value, that a switch can change its value, which switch position is the most common/important, which connections/wires are the most important for what [for function, for testing, for assembling, for repair], etc.). Or which looks the neatest…
1 Like
I also got the same idea, but…
How to make that symbols not looking for footprint but for sub-circuit.
May be you can use some from hierarchy schematic to reach the same. I never used so not sure.
1 Like
Not necessary. For an IC, you also don’t look for a sub-circuit with all the transistors. An extra little schematic with the switch circuit would be enough. It can even be placed in a corner of the main schematic if you like. The simulator might not like it, though.
For IC you want to place at PCB that IC (footprint) and not the individual transistors from it. But here you want to place those capacitors and switches. It will be not easy to tell KiCad that this symbol means 3 capacitor footprints + one switch footprint when PCB will be updated from schematic.
@pigeon
Personally, I’d leave the nine switch circuits on the page, however, I would spread them out to leave “white space” as @paulvdh suggests.
Decrease the width of TONESTACK then spread out INPUT, INPUT & TONESTACK across the page.
I’d also increase the width of the boxes a little so the labels (left) and caps. (right) are not so close to the dotted box . Likewise, the top… remove the small “input” from above the sw. and lower the SW1 & INPUT to move them from the dotted outline.
Do similar to OUTPUT & CLIPPING boxes.
Main circuit below is nice
1 Like