This is a really newbe question…
I’m running KICad version 8.02.
I want to load up and modify a complete project I’ve found on Github…
I’m complelty lost on how to get the libraries to work…
The specific project I want to play with is:
I can’t seem to get the library loaded and properly connected with the project…
It always ends up with ?? boxes in the schematic.
Schematic symbols have the wrong layout (IE don’t match the wires in the schematic)
footprint or are rotated 90 degrees…
Is there a specific tutorial that covers getting a project online and loading it up?
Can some one explain to me the EXACT step by tedious step process to get this loaded and setup directly as a local project?
Thanks you in advance for taking the time to help.
First, there is no KiCad version V8.02. I guess (but don’t like guessing) you probably mean V8.0.2. In that case you should update to V8.0.3. Increments in the third digit are bug fix updates and released approximately monthely. (Kicad is a very active project, and each month between 50 and 100 bugs get fixed.)
I had a go at that project, and for me it converts without big problems. But you have to push the right buttons in the right order.
Double click on the pecanpico10.pro file to open it with KiCad.
Open the schematic editor.
Click OK for the Not Found Libraries (They are from an old KiCad version).
In the Remap Symbols dialog, click on the Remap Symbols button.
In the Project Rescue Helper, there are 4 symbols which can not be resqued (Antenna, Conn_01x15, D_Schottky** and Micro_SD_Card_Det**. Remember these, and then click on Rescue Symbols button.
Close the Remap Symbols dialog with the Close button.
KiCad complains about The project symbol library cache file ‘pecanpico10-cache.lib’ was not found. Click on Load Without Cache File
Most of the work is already done. Save the converted schematic.
The first and second time I did this, I did not get the last message. I guess I might have used the hardware/10a version. The third time (to write along with this writeup). I used the 10b version, and this has a bit more problems. A few of the symbols now have the dreaded [??] graphics. But this is not as bad as you may think.
To fix it:
Hover the mouse cursor over one of the [??] symbols.
Press e to edit it’s properties.
In the Symbol Properties window, click on Change Symbol
In the New library identifier drop down box, click on the bookshelf icon, and find a suitable replacement.
**Press the Change button at the bottom of the dialog.
Observe whether the graphics now look ok. Repeat from step 3 if it’s not ok. When finished, Close the dialog.
Repeat for the other damaged symbols.
Do note though, that if you replace symbols, there may be subtle differences. For example a diode may be reversed, pin numbering of transistors or other symbols may be different. In the Output directory, there is a .pdf version of the schematic. You can use this as a helper when replacing the missing symbols.
It’s a few hoops to jump through, but this only happens when converting old (V5 or older) KiCad projects. This project has the cache and rescue files, which means that it’s from KiCad V5. In KiCad V6 and later, all used symbols and footprints are in the schematic and PCB files themselves, and conversion problems should be a thing of the past.
After the conversion, KiCad does leave the old files behind, but does not use them anymore, and you can delete them. You may also want to do a bit of library management afterward, but that is mostly optional. Most of the 3D models are also missing. This is normal, because KiCad does not put these in the project. You can probably fix most of these simply by replacing the symbols from the old (not present anymore) KiCad libraries with the current KiCad library version. There is a script on gitlab somewhere to archive 3D models together with a project. But this is not part of KiCad itself, and I have not used it myself.
KiCad projects from V5 and earlier are not completely self contained. As a result, the amount of effort needed to import it into a newer KiCad version varies. The project you find is pretty good in this regard, it only needs a few minor changes.
