Hello,
I am in the transition from V6 to V9, under Win 11.
I am a bit lost with the changes in symbols names both for schematic symbols and for footprints and their association.
Building it by hand and establishing an association between symbol and footprint works smoothly, but is time consuming and does not allow to reuse work done in previous versions.
Reading this thread:
Managing libraries (symbols & footprints) including private libraries.
I discovered in the last post by Mr. Piotr an idea that seems very interesting and allows to decouple our previous work from the version changes.
It requires handling private libraries and I ignore the how to for this task.
So… I will try to build my private library with this concept using the association symbol <> footprint already used and tested in my previous PCB.
Can you please point me to a suitable document to learn how to build and configure Kicad 9 libraries to enable this nice functionality ?
Be aware that it is not necessary to associate a footprint with a symbol in a symbol library. You can leave that field in a symbol blank and do the assignment when going from schematic to layout.
A reason for pre-assigning a footprint to a symbol might be that symbol is only available in one footprint or you intend to only ever use a particular package and you want to save repetitive work across projects.
But if you don’t know if you’ll use that symbol again in future, you can build up a library of symbols with assigned footprints as you go by assigning at project time, then save the symbol for future use. You can even do it after the project is done by exporting the copy of the symbol in the schematic to a library.
Naturally saving a modified symbol requires a personal library, as the standard libraries are read-only.
I don’t think there are any documents available that cover @Piotr 's method.
Basically, he created a Database using Kicad personal libraries before the Database feature was introduced to Kicad.
He stores in personal libraries: the symbol with a reference to the footprint with the value and also its footprint. eg. Res402_1K with a 402 footprint.
If he was starting now, he would probably use the Database function.
Using the “@” key and then starting to type the ID of a member will notify a member that he has been mentioned, so I expect @Piotr will join the conversation.
If you are only interested in associating a footprint with a symbol, you only need to alter the name of the symbols containing multiple footprints to reflect the footprint attached to that symbol.
eg. Res402 has a SMD 0402 footprint. Res603 a 0603 footprint.
To do this, open the symbol in the symbol editor then attach the required footprint using the Symbol Properties (through File, icon or assign a hotkey).
There is also some information on library manipulation in the FAQs. see Beginners Guide and Tips & Tricks.
No!
Not exactly. You don’t have to reflect footprint in name provided you use more libraries.
You describe conception I was using with Protel (we bought Protel 3 in 1997 and were using it till I moved in 2017 to KiCad).
The main assumption was to be able using only the symbol name to select all rest element information (to make BOM) from spreadsheet (first tab contains database, second tab makes BOM by using functions allowing to select fields from first tab).
The other was that use of new R value needed to design new symbol so it was the moment to consider once more if we really want to extend number of drawers to store resistors or may be we could use some of values we already store.
In Protel symbol names meaning was:
1k = 1k 0603
1k_4 = 1k 0402
We used UniversCondensed font to have the names at schematic not too long.
When decided to move to KiCad (4.0.7 was first I tried) I found that I can’t use UniverseCondensed font and names are too long. As practically to understand schematic I don’t need the information about footprint so I decided that both 1k 0603 and 1k 0402 can at schematic have the same symbol name: 1k.
I have checked if I will be able to make my spreadsheet database serach not only by symbol, but by symbol concatenated with footprint and found it is possible.
The problem is that KiCad don’t allow to have two symbols with the same name in the same library.
Because of this I have library R and there 1k means 1k 0603 and library R1 (from 1mm length) and there 1k means 1k 0402 and library R2 (from 2mm length) and there 1k means 1k 0805. The same with capacitors.
For ICs I don’t use the same symbol for different packages. At first selection of some IC I use its short symbol name assuming that the case we use are just default for us. For many ICs it is the end - we never use it in another case. But recent problems with ordering elements forced us to use what was available at the moment. The effect is that I have in library:
HVD72 - combinded case SO8 + VSON8
HVD72D - SO8
HVD72DGK - VSSOP8
HVD72DRB - VSON8
It is the only IC I have in library 4 times. Most others I have only one time in library.
I am repeating information that I have already written. Here are the previous posts with full explanation (and examples) of my BOM generation I have designed in ‘Protel times’ and modified when were moving to KiCad.
You made me to learn how to search anything in Forum. Never did it.
I see that those my last post is not about having symbols linked with footprints but only about having your own libraries.
When deciding to use only my own libraries I didn’t know that thanks to that it will be easier to move to next versions. For me it is ‘side effect’.
The problem is that when you use your libraries and KiCad libraries (I am speaking only about global libraries - I have never tried to use project specific library - don’t see any advantage in it) then with new KiCad version the new libraries come and you have someway once more mix your library list with KiCad libraries. According to what I have read there is still no automatic way to do it.
As I use only my libraries my library list stays not changed.
The only problem I have with version change is that when at first run I specify that I want to use my library list KiCad asks me to let him know that list and opens window (I use Win10) to point the file containing the list but that window doesn’t show hidden/system files. So till now before doing it I just had to copy KiCad library list files somewhere to be able to point on them. and had nothing more to do.
How with V9 I don’t know. If I will have to do any PCB now I will use V8 for it.