Empty Property Name error while opening schematic in Kicad

[Jayesh1]

Hey there, I am using Kicad 7.0.2. I am not able to open my schematic file in Kicad, it show error like: “Empty property name in “file path” in line 20XX, offset 16.”
Whenever I make a new schematic, it runs for the first time, but when i try to launch it after closing it, this error occurs. I tried opening the file in text editor and the property fields are empty. I have no idea what to put it in there. Anyone have any solutions for it?

[gmc]

Can you post the version info. Help / About KiCad

Are you able to zip the project and attach here (If it’s not confidential)

Guessing here, but can you try a folder without a space in it (I can’t imagine that the issue but worth ruling out)

[Jayesh1]

Here is the version info :
Application: KiCad x64 on x64

Version: 7.0.2, release build

Libraries:
wxWidgets 3.2.2
FreeType 2.12.1
HarfBuzz 6.0.0
FontConfig 2.14.1
libcurl/7.88.1-DEV Schannel zlib/1.2.13

Platform: Windows 11 (build 22621), 64-bit edition, 64 bit, Little endian, wxMSW

Build Info:
Date: Apr 15 2023 19:18:27
wxWidgets: 3.2.2 (wchar_t,wx containers)
Boost: 1.81.0
OCC: 7.6.3
Curl: 7.88.1-DEV
ngspice: 40
Compiler: Visual C++ 1934 without C++ ABI

Build settings:
KICAD_SPICE=ON

[Jayesh1]

Here is the link for zip of the folder… what do you think the issue can be?

[gmc]

I’m getting the same issue on 7.0.2 in Ubuntu.
The issue is being caused by this field in the .kicad_sch file (Actually a number of components with the problem)

    (property "" "COM-09426" (at 228.6 74.295 0)
      (effects (font (size 1.524 1.524)) (justify left))
    )

The property value is empty causing the crash. Might be worth raising a bug for this.

As a workaround you can edit the file with a text editor (make a backup first) and remove the 3 lines. (I’m not sure what the property should even be) You will have to search through the file as the empty property appears a number of times.

[ratsnest]

Are these parts coming from a legacy .lib library? Try migrating the library to the new .kicad_sym format in the library manager. That did the trick for me.

[pisozo]

Hello All, I am also having the same issue.

I ended up opening my .kicad_sch file in Vim and I found the property as shown above. After looking around before and after this code it seemed to be a component instance and the property which was causing an issue was an unnamed field in the Symbol properties. I edited it to reflect the right Field title and the problem went away. The project opens with no problem.

I guess the issue has to do with legacy vs. 7.0 KiCAD. Legacy seems to have dealt with unnamed symbol property fields better than 7.0.

[pisozo]

I tried this but the issue was still there. Maybe it would have worked if I was also able to update the SCH with the newly migrated components. I think lesson learned is migrate your .lib’s first then include newly migrated components into the new KiCAD schematic.

[ratsnest]

Oh, yeah. You’ll need to manually delete the old part from the schematic using a text editor. Then add it back in after migrating the library.

[pisozo]

Actually, I didn’t manually delete the part using the text editor, I used the text editor to fill in the missing property field name.

I.e.

    (property "" "COM-09426" (at 228.6 74.295 0)
      (effects (font (size 1.524 1.524)) (justify left))
    )

changed to:

   (property "Manufacturer PN" "COM-09426" (at 228.6 74.295 0)
      (effects (font (size 1.524 1.524)) (justify left))
    )