One person recommended not using standard (master) library symbols at all in the schematics - that is, they should all be copied/edited to a customs Symbols folder. If any of you could point out what it is I should look for or consider in doing this ?!
as well, I noticed symbols have pins notated with numbers - I’m assuming these are required for the netlister. Otherwise can these be changed to letters ?!
If you use something other than numbers they will not match up with the standard footprints supplied in the KiCad library so you would have to have different footprints too.
Well one possible angle: If you use all your own footprints and symbols (I think I am doing that) then theoretically there is no chance of your symbols or footprints changing when you update your KiCad version. I don’t think there is much changing (of existing symbols and footprints) going on in the standard library but I am not certain.
If you like something which is in the standard library, then just copy it into your own library and it should not get changed unless you change it. As for me, I have put my own personal preferences into almost all of the symbols and footprints that I use.
One thing to remember is that most IC packages are common to different devices. A 14 pin TSSOP will be used for quad op amps, quad comparators, and a digipot that I am using. If you assign pin names which suit the quad op amp, they will be all worng 
for the other devices using the same package.
Many years ago we decided that we use in documentation (among other) 2 files. Both containing Edge.Cuts, dimension lines, CrtYd rectangles on the background of gray copper. One file having references and one having values. When you have a matrix of 0603 resistors and capacitors placed touching each other you have no place for reference and value at one picture.
In Protel 3 to get these pictures it was a complex process and I often made mistakes which resulted in doing everything again. It was the reason that when I started to be interested in KiCad (4.0.7) first for what I was searching was a simple way to get my documentation files.
I found that using standard library footprints I can’t get it so my decision was - I will have my own footprints. I don’t know if starting now with V6 my decision would be the same.
And about symbols. I am just used to have in library only symbols of selected to be used elements with everything defined (value and footprint). So I know that when I place element at schematic I just need not worry about anything and I can’t make mistake when assigning footprint (I have never even seen how the process of assigning footprints look like). So in my symbol library I have resistors with specified values. If I need new resistor value I don’t change it at schematic but I add new alias in library (still in V5) and I also add that resistor to my spreadsheet I use to generate BOM. I found that I can have two resistors with the same value in libraries provided they are in different libraries. So I have library R with 0603 resistors (standard we use) and library R1 with 0402 (R1=1mm) and library R2 with 0805 (R2 = 2mm).
Hope it will help you.
I think I was the one mentioned by the OP recommending copying/editing into personal libraries with these comments:
These, for example, are my personal thoughts on symbol libraries:
I sometimes don’t like the size and shape of the rectangle.
The pins are too long for my liking.
The pins are sometimes in the wrong location for what I consider to be an easily readable, aesthetically pleasing schematic.
I suppose old habits die hard. I started using EDAs in the late 1980s? with Protel for DOS, for use on MS 3.1.1. The whole schematic program, including libraries, was on one floppy disc. Needless to say, libraries left a lot to be desired… you wanted to draw a schematic, you started by drawing symbols.
Not a huge amount has changed. I think I read somewhere on this forum that Kicad boasts some 17,000 symbols. I wonder how many million symbols for parts exist world wide. Most are missing from Kicad libraries… even 40 year old SMPS controllers LM3524/5 or 20 year old TNY267s are not there, and if you want pre-assembled modules you are on your own.
I have absolutely no complaints with the Kicad libraries whatsoever, I’m just pointing out that if you want to draw schematics and layout boards, making symbols and footprints and storing them in personal libraries is pretty much mandatory.
Modifying existing easy stuff and placing that stuff in personal libraries is a great way to familiarize yourself with the process, and if you place your well organized libraries at the top of the library browser it can save an awful lot of time searching and scrolling.
I use shorter pins (as short as can “work”) and smaller text (0.03 inch height.) I also delete the circles around transistors, and I like to pack my schematics as densely as possible. It seems reasonable to me that smaller text works better with short wires and denser packing. Longer wires might work well with larger text.
my “pet peeve” is a schematic with low-medium complexity but which is spread out too wide with long wires on a large sheet. Where dense packing would allow you to see and read everything in one view, this spread-out schematic requires you to scroll and zoom more than necessary.
Often a schematic is too complex to allow reading everything in one view, but spreading it out too much still wastes time when viewing it.
I’m at the other pole: I minimise my use of custom symbols and footprints, and only make them when nothing in the standard libraries is suitable. Reason is I tinker for fun and my schematics and PCBs have only to be tidy enough for me to read, no thought for posterity who will have no interest in my designs. As I tell my friends, if you look up lazy in a dictionary you’ll find a mugshot of me.
All the same you’ll need the skills of making or modifying your own symbols and footprints because it’s inevitable someday you will not find a suitable one in the libraries or online.
I don’t think you would be on this forum if that were true.
I guess more than anything, I want to easily read my own schematics. To heck with posterity and to heck with posterior for that matter.
So on what would I be expected to sit to view this forum???
Agree!
FYI:
Some considerations:
• I work on projects within my interest, that eliminates 98% of the included Symbols and Footprints
• I set the ‘Manage’ Symbol and Footprint panels to Load Only the 2% I do use. Thus, faster loading and reduced (un-cluttered) listing of items I don’t use.
• I have several custom folders for my Footprints and Symbols - they are not accessible to Kicad default Path. Thus, not affected by Kicad updates…
My custom folders… (in my Home User Directory)
Another reason you could want to use your own libraries is the option to add more information to the symbols. Per kicad library convention it is not allowed to have information like MPN, distributor part numbers etc. in the standard libraries schematic symbol and therefore you either have to add these information later per hand to the schematic or use third party scripts to get them in there.
Connected to this is also that you may want to use a different approach on how you structure the symbol library. The standard library only offers generic symbols for some groups of components (like caps or resistors) so you can’t search for something like 10k in your library to add it into the schematic. So I use for example dedicated libraries only for caps and resistors of different sizes where all caps and resistors are stored (with more detailed information) I ever used with KiCad.
Thank you all for your useful replies.
I thought I’d give the forum a break and jump back into the program - I just finished two board designs recently, one tiny one not so. I’m really enjoying the intuitive feel of Kicad6 btw.
I’ve had another good chance to see what it was like doing things from scratch by using the standard symbol library and adding the extra info as Tojan last stated here. I can see the usefulness for managing custom symbol libraries, if only to save time filling info repeatedly, etc.
But, still after going through the docs I’m having a hard time managing the folder I created and the symbols I put in there. I think I might have copied stuff over wrong or simply without thinking about what I was doing. Either way, I’m confused by the fact that my custom_symbols folder has kicad_sym entries that show as one-item folders in my Symbol Library Browser and some as nested folders even though they are single text files in my custom symbol folder.
I will likely blow this folder away and start over once I know what the proper Custom Symbol library creation process is. Maybe some of you can explain how you go about doing this …
(sorry if this sounds lame)
TIA
I think you run into a mix of heritage v5 symbol libraries which put all symbols of a library into one large text file and new v6 symbols where each symbol is its own file. I recommend you to convert the v5 libraries to v6.
For the custom libraries grouping I usually group them after function/part group. so I have a library for power-management ICs, a library for inductors, another one for diodes and so on. A bit special is maybe the way I handle resistors: I create a library for any resistor size I use because like this I can use multiple resistors named “10k” in parallel as kicad differs them by the library name.
Hello @kicadian
Start by creating two folders with your operating system, NOT kicad.
Name these eg. My Kicad Symbols and My Kicad Footprints or whatever you prefer.
Next, open Kicad / Schematic Editor / Create, Delete & Edit Symbols
Up comes Symbol Editor.
Click File / New / Choose “Global” and OK.
Up comes a “New Library” screen…
Next, give your library a name.
Click on Other locations to find the symbol folder you created.
Highlight that folder then save.
Repeat this for as many libraries as you require.
Note: think about your naming of libraries and how many and what goes in them.
I have 15 different symbol libraries.
@BlackCoffee shows you his examples.
You can add more libraries as you wish in the future.
Next, you have to show the paths of these new libraries you created to kicad.
Go to Preferences / Manage Symbol libraries / click Global then the Folder icon…
Now you should have a list of new empty libraries probably at the top of kicad list.
Finally!!!
Open up your Symbol Editor again, scroll through your existing personal libraries, find each of your personal symbols and, one at a time, right click it, select “save as” then in the new “save symbol as” window, scroll through the library list to find the new, correct library in which you want the symbol placed, change the name of the symbol only if you wish then click save.
Repeat as required for all your personal library symbols.
Not lame, and if there is something from the above you do not understand, please ask.
One more thing: footprints work exactly the same way, just substitute the word symbol for footprint in the above and place your new footprint libraries in the footprint folder you created.
We, or i since i am the only one creating PCBs in our company, use only our own symbols and footprints. The reasons:
Not true! This was the preliminary plan before the new file format was implemented, but for practical reasons it was not realized. Each file is still one symbol library.
KiCad doesn’t care about folders when we talk about symbol libraries. All that matters is that each library (file) is in a library table (either the global one or the project specific).
Ah ok. as I still work with v5 I did not saw the final implementation yet. I crossed out my comment on this.
Thanks for your replies all …
so, let me get this straight - Kicad uses the term library in vastly different ways, including in reference to a schematic symbol ??! … and also, in reference to a collection of schematic symbols ??!
also, WHERE does the official documentation cover all this file structure stuff ???
Thx!
https://kicad.github.io/symbols/
Symbols
The KiCad symbol libraries are the individual
.libfiles, with the corresponding.dcmfiles containing symbol metadata. These symbols are best used in combination with the official footprint libs.Requirements
The files packaged here are intended for KiCad version 5 or nightly builds that support the schematic library version 2.4 or newer.
page 6 needs filling in here 
found it, well some of it …
https://docs.kicad.org/6.0/en/eeschema/eeschema.pdf
at the bottom of page 85 …
This I find confusing …
Symbol Library Editor Overview
The symbol library editor main window is shown below. It consists of three tool bars for
quick access to common features and a symbol viewing/editing area
maybe I’m being pedantic here, but shouldn’t that more simply read only as Symbol Editor ?!
Maybe, maybe not. My gripe about usability of that editor has been that it tries to do two different things in one UI, namely editing individual symbols and organizing symbol libraries. So you can’t know which main menu item belongs to which task. For example “Copy” may mean “Copy symbol from library” or “Copy item inside symbol”.
