In Kicad 6 Is there a way so that the symbol name and the symbol value may be different? I would like to give a name to a symbol so that it is linked not only to the footprint but also to its characterisitics. For example I would like to name the symbol as: C-100nF-50V-10%-0603 and value as: 100nF/50V, the reason is to don’t fill the schematic with “strange” values or with more information then needed. Now, to have this result I added a custom field (val) and I have to put it visible and the field Value invisible. In practice I prefer to have multiple capacitor symbols, one for each capacitor I have in internal warehouse to simplify the inventory and assembly process.
These have been separated in v6.99, i.e. in v7 in the near future, but not in v6.0. Currently the only workaround is to add another field used for the value.
In Kicad 6 Is there a way so that the symbol name and the symbol value may be different?
Not in the symbol-library, there is the requirement symbol name == symbol value.
Afterwards in the schematic you can change the value to any other string.
If you wait until v7 (or start using the nightly development versions): than you are free to write symbol names different from symbol values.
Perhaps this may help (at least with keeping it clean)…
This is what I do as I don’t like more info than I need…
• I locate a Symbol of interest (or make a new Symbol)
• Save_As (save with the same Text that I’ll use for the Value)
• Edit the Value’s text (to be the same as I saved it as) - USE a ‘Dash’ at the end, this will update with the Number of the item in sequence if there are multiples
• Hide Visibility of the Value
• Show Visibility of the Ref
My symbol library will list the items by the Ref which is the Value info I entered
Now, I can place the Item and it shows only the graphic and the value (with the specific Number of the item if multiples…)
Bingo!
Screenshots of the Cap’s I frequently use and the fields in the editor
I think this is the wrong approach. You will create a maintenance hell by doing this, unless there is some solid base behind it.
Edit: Oops, this response was directed to the first post of aiotech-massimo, not at BlackCoffee.
These database driven libraries are probably a better option:
If referring to my approach, you’re correct with respect to the standard/default Kicad Lib’s.
But, I place all of my Symbols, Footprints and 3D-Models in personal folders (on the Path) so, Kicad always sees them and won’t mess with them.
If not using personal folders, then, ‘yes’ probably not a good idea to use my approach. But, we’ve (meaning many of us at this forum) use personal folders for our Symbols, Footprints and 3D-Models… (as I’m sure you know and perhaps also do)…
I’ve seen so many contortions on how to do this, it sometimes makes my head spin.
The basic issue is, that the KiCAD symbol library is a:
Symbol Library!
It’s not a component/parts library, and is not really designed to be used as such.
There are other EDA packages that will handle this, downside is you’ll need to get your wallet out of your pocket.
1 Like
If you design professional PCBs you do not want to edit every time the symbol list to associate packages and M. P/N, having boards with hundreds of components it is a time consuming activity and increases the probability to make errors.
I use the same system to define component names but I add the VAL field to put the minimum needed info on the schematic. So, I will wait for 7.0 and live with the VAL field for a while.
I will wait for 7.0 and in the mean time I will live with the VAL field.
I have such capacitor with name=value=100n50 to have it as short as possible. In Protel I used Univers Condensed font. When migrated to KiCad I found that ‘/’ can’t be used in name so I don’t have it (may be I didn’t noticed that it is now possible).
Previously (in Protel) I assumed that the name fully identifies a part - so I had 1k for 0603 and 1k_4 for 0402. In KiCad I decided that name+footprint fully identify the part so both 0603 and 0402 have the name 1k (I had to have them in separate libraries).
For most capacitors (1n, 10n, 100n) I use only value what means for me that voltage don’t care. If voltage cares it is in symbol like 10u50.
The full descriptions (like 100nF-50V-10%-0603) I add using LibreOffice spreadsheet containing database of all elements I use (value concatenated with footprint is used to select the right element from database. Database is simply one sheet in spreadsheet and BOM is generated at second sheet by searching (automatically) descriptions from database. That way I can list several elements to be used for specified part. Something I entered to my spreadsheet few days ago:
EC2_12 with footprint EC2 is described in BOM with 3 lines:
Kemet: EC2-12NU (EC2-12NJ)
Hongfa: HFD3/12
Omron: G6S-2 12VDC (G6S-2-Y 12VDC)
Yes, you wrote that twice. 
As an alternative, you can already install KiCad-Nightly V6.99 and at least start experimenting and learning how this new database part of KiCad works. It’s likely to have some bugs as it’s a brand new feature. As an early adopter of this feature you may also have more influence over it’s implementation, and it’s also a way to give back to Kicad if you can help with tracking down bugs and reporting them.
Ciao Massimo,
i was previously going to suggest you to have a look at the database-library workflow, but reading your quote i deleted the answer since the dbl workflow is in fact the exact opposite of your preference.
reading further replies i still think that you should at least try it, since probably it answers all you needs, just in the completely opposite way you are used to do now.
Well, the reason because we draw a schematic is to produce a PCB or a simulation and rarely it may be the same for both. So, from a logical point of view, we should organize a component/part oriented library but it is a total different paradigm then those implemented in Kicad 6. A part should be identified by a part number linked at least to a symbol, a footprint and a datasheet. I think this way is the best possible.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.