Libraries missing open KiCad 5.0 project in KiCad 6.0

[Hans_Bos]

I whould like to creat an Arduino shield for the ArduTrx project.
the KiCad 5.0 files are available at: http://ardutrx.generationmake.de/ArduTrxShield_1.1.zip
But.
After opening the KiCad scematic project in version 6.0 I get the problem with libraries that are missing:
The list is found below.
How to solve this???

ATX_connector.lib
CAN-transceiver.lib
come_connector.lib
CON_wuerth.lib
D_esdprotection.lib
devices.lib
displayport_connector.lib
displays.lib
electrical-connectors.lib
eth_usb_connectors_combos.lib
ftdi.lib
IC_batterycharger.lib
IC_clockbuffer.lib
IC_interface_i2c.lib
IC_levelshifter.lib
IC_loadswitch.lib
IC_microcontroller_ST.lib
IC_rtc.lib
IC_sensor.lib
IC_transceiver_can.lib
IC_transceiver_rs.lib
IC_usbhub.lib
interface.lib
LED-controllers.lib
L_filter.lib
L_power.lib
mechanical-connectors.lib
mechanical-switches.lib
MECH_smd-contact-finger.lib
MECH_smd-mounting.lib
MECH_smd-spacer.lib
MEMS.lib
microcontrollers.lib
MODULE_compute.lib
motor-driver.lib
opamps.lib
PCB_touch.lib
PCIe_connectors.lib
power-monitors.lib
power-supply.lib
sata_con.lib
transistors.lib
usb_connector_header.lib
voltage-regulators.lib
MODULE_RF.lib
IC_audio.lib

Thanks
Hans

[paulvdh]

I also get that long list of missing libraries, but this is sort of expected when loading a project from an old KiCad version and it should not be a problem.

Looking at the files with a text editor, the schematic begins with:

EESchema Schematic File Version 4

and this “file version” does not mean much to me. However, the PCB starts with:

(kicad_pcb (version 20171130) (host pcbnew 5.0.0-fee4fd1~66~ubuntu16.04.1)

KiCad V5.0.0 is quite old but KiCad V5 already has the Cache & Rescue mechanism, and there is a [Projectname]-cache.lib in the project, but unfortunately it is very incomplete. It only has a single “Wurth” connector, and that is the only part that can be rescued.

The best thing you can do is to contact the orinal author, tell him the project is damaged and if he is willing to repair the project. If he still has the original libraries installed, it could be a simple process to re-generate a complete [Projectname]-cache.lib file, There is some contact info at the bottom of his web page:

If you have any questions contact me via email at bernhard@generationmake.de, make an issue at github or send me a message at twitter (https://twitter.com/generation_make).

Apart from the [Projectname]-cache.lib file, the project is fairly complete. You can create links to new schematic symbols in the schematic to get rid of the [??] graphics. (Do not delete those symbols, only edit the library links!). You can use the .PDF version of the schematic to do the repair. It’s a tedious job, but it’s also quite straight forward. You do this with: Schematic Editor / Tools / Edit Symbol Library Links.

In the screenshot below, I replaced all “R_1206” resistors with a default “Device:R” resistor from KiCad’s standard library.

Which immediately shows up in the shematic:

But they’re a bit too big. A second replacement with R_Small appears to fit, but I don’t like those small resistors personally.

You’ll have to repeat this for each type of symbol.

---

Also, I see there is also firmware for this thing on github. The orinial author may be interested if you send him a merge request or repaired project.

[paulvdh]

Another way to repair groups of symbols is to first select one of the dreaded [??] symbols, then press e to edit it’s properties, and then use Change Symbol from the symbol properties.

After having repaired only resistors, capacitors and GND symbols, some parts of the schematic are already beginning to look normal:

[paulvdh]

Addition:
There are three reasons to repair the symbol links instead of replacing them with new symbols.

1. You can do a whole group of symbols in one sweep, which is much quicker then one-by-one.
2. It preserves the values of resistors and capacitors. Resdef, etc.
3. It preserves the link to the PCB footprints.

The dreaded [??] schematic symbols look really awful, but it’s just the looks, and don’t be intimidated by that. Except for the graphics, all the other information is still present.

It’s also important to note that starting with KiCad V6 this info is embedded directly in the schematic itself, and newer projects will never get damaged in this way.

[eelik]

@Hans_Bos

devices.lib

KiCad doesn’t have this library even though the name resembles the current official Device library. Maybe the design was originally made with even older than v5 (see kicad-library/device.lib at master · KiCad/kicad-library · GitHub where the last commit is made well before the 5.0.0 release). But many of the libaries can’t be found even in the old repository. There’s nothing to do if the libraries haven’t been published. I tried the rescue process but it doesn’t help.

[paulvdh]

I think KiCad’s library names changed from plural to singular in the transition from V4 to V5, but it won’t help as many of the symbols appear to be modifications. For example I saw a lot of “R_1206” schematic symbols, and I assume these have a 1206 sized footprint already assigned in the library, but that also makes them non-standard.

@eelik

I tried the rescue process but it doesn’t help.

Indeed, there just is nothing to rescue. But that does not mean it’s hopeless, especially with the .pdf versions of the schematic it’s relatively simple (though a bit tedious) to repair. I guess it can be done in about an hour of work, maybe two.

[Hans_Bos]

Thanks for the support. I started making my own symbols and footprints in KiCad 6.0
It’s my first KiCad project so it will be something of a challange to me.