Should the schematic reflect the circuit or the layout?

[Yuu]

This may sound like a silly question but after designing a couple of boards in Kicad, I've come across situations similar to what you see below:



As you can see, in my schematic, I use the 1x1 connector socket symbol because that reflects the actual PCB I'm making. It makes it super easy to assign the pre-made footprint.
However, the actual components I'm putting there are just resistors so at the same time, I would like a schematic that shows resistors instead of the socket symbols. If I did that though, I can't assign any pre-made footprints that have two 1x1 sockets. I would have to make a custom footprint. That's not a big deal because I already do that for plenty of things but I'm curious on what is proper? Do you put the sockets like I've done? Do you put resistors? Do you somehow show both in the schematic? Do you make two schematics?

If it was TH or SMT, I put the resistor symbol of course but I'm not sure what is best for off-board connections/sockets/etc.

[thm_w]

Lazy solution would be to just draw the resistor symbol there where it is connecting, and have it as graphical only.

If the end result is them being populated, IMO, the proper thing is to have a custom symbol, that shows resistor and socket together. Then with that you can't screw up by placing J2 beside J10 on the PCB and having it go to the wrong place.

[Yuu]

Ah that's a good point. I had somewhat forgotten you could create custom symbols.

One thing that made me think about this topic was seeing a schematic of someone's lofi noise box. In the pic below, you can see he denotes the potentiometer R49 is external to the board by placing it between the X15 and X16 labels. I think that's sloppy and hard to recognize because they look like net labels instead.


If I had to make a schematic where an external potentiometer is soldered to pads on a circuit board. I'm not sure how I would do that yet. I wouldn't make a custom symbol with socket symbols because that would just look funky. Maybe mounting hole symbols on each end of the potentiometer symbol. Nothing satisfying immediately pops into my head. Would have to think about it later.

[thm_w]

Most would just have the potentiometer symbol as in a normal schematic. You can look up some audio amp schematics, or old PSU schematics that use multi turn pots.

I agree I don't like the X15 mark, I think a normal pot symbol is better, and then a normal symbol with some note or additional markings showing its panel mount would be best. Then for soldering, silkscreen labeling with wire colors or designations on the PCB. But different people/companies have different preferences.

[CatalinaWOW]

Simply placing the pot in the schematic causes another problem.  It will create a part that needs placing on the PCB.  As near as I can figure the best approach is to create connection points (connectors, solder eyes or whatever) for the pot that will then be placed in the PWB, and then use a symbol with no footprint for the pot.  That is still likely to give you an issue at BOM time.

[Doctorandus_P]

The first and most important goal for the schematic is to have a user readable reference of what a circuit does and how it works.
The schematic is all about function, and not about form.

For you as the designer it does not matter much (at the moment) because you've probably put a bunch of hours into designing it and know every detail intimately.
But what if someone else reads it, or if you want to make a modification 5 or 10 years later?

For the function it does not matter at all whether a (power?) resistor is soldered directly to the PCB or via some connector. But if you do not even show there is a resistor in your circuit the schematic is broken. I have no idea how many and how the resistors are intended to be connected to your connector. I could guess there would be 4 resistors, horizontally connected, but it's a guess, and I don't like to guess. Your schematic also does not show the value or power rating of the resistors. It's not even in your BOM so you probably forget to order it.

The schematic of the "lofi noise box" is the expected and normal way to draw a schematic. For the function it does not matter (except for some parasitic inductance / capacitance) whether the potentiometer is somewhere else. If you want to be explicit, then you could draw a dashed line around it and add a comment that the potentiometer is off-board, but I regard that as mostly clutter and implementation details that obfuscate the function.

It really should be big things first. And the big thing is that there are resistors in your circuit, and how they are connected to the rest of the schematic.

Similar for IC's. When I see a circuit in which all the pins are drawn in the order they are on the IC, then my first question is "does this make sense here?" and almost always the answer is no. (Sometimes it makes sense, for example for a test socket in an universal programmer). Another example is showing operational amplifiers as a square box instead of triangles, or even worse, a quad op-amp which has a single dip-14 schematic symbol. Yuch! When I see those things, I rarely look further at the rest of the circuit but just post a remark to redraw the schematic. I am just not willing to waste time into deciphering such stuff.

[Yuu]

Thanks for the reply Doctorandus. Makes a lot of sense.
It's funny. I had socketed op-amps in that same circuit but I used the op-amp symbol in the schematic and just set the footprint to the socketed one. Not using the op-amp symbol, and instead using a box with 8 pins, would be very cancerous and make the schematic unreadable.
In the future, I'll use the regular resistor symbol. Then I can just make a custom footprint. As far as BOM stuff goes, I can add as many digikey attributes to a symbol as I need. Works great for personal projects but likely slightly improper for formal situations.
I looked at some older schematics at work today and they use dashed lines to indicate whether components are external or not so I think I'll adopt that when I feel it bugs me.

[Smokey]

Another thing to consider is that if you are generating your BOM from your schematic, then you will need to remember to add those resistors to a higher level assembly BOM somewhere or they won't get purchased.

Another sort of related problem I've run into is with something like the Raspberry Pi CM4 module.  I have a single CAD part that represents that module as one thing (mounting holes, connectors, outline, etc).  But the actual parts that need to go on the PCB BOM are two individual SMT headers.  This screws up the pick and place file because it only shows one part with a central pick point, not two separate connectors each with their own pick points. 

[JohanH]

Simply placing the pot in the schematic causes another problem.  It will create a part that needs placing on the PCB. 

No. Just assign three holes as footprint to the potentiometer symbol, or a three pin terminal, connector, whatever you use to connect the potentiometer to the PCB.

Also, you could create a whole off-board part of a schematic and mark the parts as not to be placed on the PCB (in the symbol properties). For clarity, add some graphic and/or comment that makes it clear they are not part of the circuit board.

[Yuu]

Another sort of related problem I've run into is with something like the Raspberry Pi CM4 module.  I have a single CAD part that represents that module as one thing (mounting holes, connectors, outline, etc).  But the actual parts that need to go on the PCB BOM are two individual SMT headers.  This screws up the pick and place file because it only shows one part with a central pick point, not two separate connectors each with their own pick points.

Yeah I can see things getting a little tricky if you're using pick and place and not just hand soldering all the parts. I haven't had to delve into that yet since I've just been doing personal small stuff at this point.

[shapirus]

FYI the image isn't loading for me, probably because imgur doesn't like my proxy server. The error code is "429 Too many requests".

This is an example why hotlinking images should be avoided.

[Yuu]

Hmm, I figured imgur is the cleanest option because then the images are inline. It looks pretty to me. I prefer it over having it as an attachment and then having to click them and what not.
I wasn't aware imgur doesn't work for some people.

[langwadt]

Another thing to consider is that if you are generating your BOM from your schematic, then you will need to remember to add those resistors to a higher level assembly BOM somewhere or they won't get purchased.

Another sort of related problem I've run into is with something like the Raspberry Pi CM4 module.  I have a single CAD part that represents that module as one thing (mounting holes, connectors, outline, etc).  But the actual parts that need to go on the PCB BOM are two individual SMT headers.  This screws up the pick and place file because it only shows one part with a central pick point, not two separate connectors each with their own pick points.

the CM4 module is iffy anyhow, the connector datasheet specifically says to only use one because the mounting tolerances for mounting more is +/-0 i.e. impossible

[shapirus]

Hmm, I figured imgur is the cleanest option because then the images are inline. It looks pretty to me. I prefer it over having it as an attachment and then having to click them and what not.

Yes attachments in this forum engine suck. That's why I use a (somewhat tedious) workaround of opening them in a new window, then editing the message and copying the image URLs and pasting them back enclosed in the img - /img tags. That saves them on the server(s) along with the forum's data and they work for a given visitor whenever the rest of the forum works.

I wasn't aware imgur doesn't work for some people.

I wasn't aware either before I started to notice an occasional missing message in some posts . Apparently they treat my proxy server's subnet block as "bots" and respond with a 429 regardless of whether my specific IP address has ever done anything bad or not. Which sucks.

[Smokey]

Another thing to consider is that if you are generating your BOM from your schematic, then you will need to remember to add those resistors to a higher level assembly BOM somewhere or they won't get purchased.

Another sort of related problem I've run into is with something like the Raspberry Pi CM4 module.  I have a single CAD part that represents that module as one thing (mounting holes, connectors, outline, etc).  But the actual parts that need to go on the PCB BOM are two individual SMT headers.  This screws up the pick and place file because it only shows one part with a central pick point, not two separate connectors each with their own pick points.

the CM4 module is iffy anyhow, the connector datasheet specifically says to only use one because the mounting tolerances for mounting more is +/-0 i.e. impossible

Yup. 
https://www.eevblog.com/forum/manufacture/fine-pitch-high-speed-connector-alignment-issues-(ex-rpi-cm4-headers)/

[babysitter]

I put a lot of comments in schematics, boxes for parts that should go together or in a certain place, and if a wire needs special attention, it will be thicker, e.g. when carrying power or should be really, really short. Must confess, I might still be more accurate.
BR