Importing project from V5 to V8

Software
1

Hi, I’m upgrading from an old V5 install of Kicad to V8. I’ve ran into a couple of problems and am hoping to get some advice.

  1. When I open my schematics I see that some of the reference designators are missing.
    These were complete and working schematics in V5 - I’ve even had them manufactured.
    I can open the V5 schematic in a text editor and find that the reference designators are present.
    I saved the schematic in V8 and opened it in a text editor. When I find one of the parts, I can see that the designators are missing. They seem to only be missing on hierarchical sheets and then missing only some of the parts on some of the sheets.

  2. I’m also getting two description fields in the properties of each part - only in the schematic. Again, when I open the schematic in a text editor I see an extra field now called description_1.

2

I recommend opening an issue in GitLab and attaching your project to it. You can copy and paste the content from your post.

Issues that include conflict files are highly valuable to developers. This way, they can identify the source of the problem and, with some luck, patch it in the next bug release.

Best regards,
2nOrderEDO

3

Not sure if related to it.
In V5 symbols used at schematic were not included in schematic file, but were in separate file (sorry don’t remember its name). I always deleted that file, as I use only my own libraries so links to symbols are valid after I change KiCad version.
Since V6 symbols used in schematic are included in schematic file so even library is not available schematic has everything needed.

4

See this issue, with the fix going into the next “Testing” build

1 Like
5

Yes, as @davidsrsb posted, this is a bug in 8.0.5 that is fixed for 8.0.6 (not yet released)

As a workaround, you can first migrate your project from V5 to V7, then from V7 to V8. This should prevent the problem.

1 Like
6

Yes, very big jump version upgrades are basically under-tested, as so few people do this.

7

Hiya, Thanks very much. Yeah I thought I’d be pushing my luck with such a big version jump.
I had a look at issue #18779 and it looks like it has been completed for the 8.0.6 milestone.
Is it worth trying the nightly build? My projects are more professionally oriented rather than hobby, so I’m pretty keen to not bork them. In not, I’ll try the V7 → V8 approach. Thanks again

8

If you use the 8.99 builds you will not be able to work with them subsequently on 8.0 bulls.

9

Nightlies are “V8.99” and experimental. You want to stick to “Testing” which is what will become 8.0.6 and still “V8”
The “8.0.5.71” build should contain the patch

10

This. But please back up your projects before importing in case there are further issues, or unknown issues with the testing builds.

1 Like
11

The merging from V5.1 to V6.0 was a major leap with lots of changes. 6.0 to 7.0 to 8.0 are more evolutionary.
My recommendation would be to install V7.0.11, which is the most reliable version I’ve worked with in the last years. It’s also the best documented. After that, a migration to V8 is easy.
Very important is, that you preserve your 5.1 symbol/footprint/etc. libraries. They are NOT part of your design files except for a reference. In V7, you’ll have to open each schematic separately and update the symbols (they may have changed) to integrate them into the new schematic files.
Tedious, but necessary.

1 Like
12

Thanks for the clarification on Nightly vs Testing.
I definitely backup my projects and libraries!

13

I’ll try the Testing approach with one project and see how it goes.
If I don’t have any luck, I’ll give the V5 → V7 → V8 method a try.
I’ll let this be a lesson to not snooze on my updates…

14

If you get errors with the patched V8.0.5++, please submit an issue so that the developers can have a look. There is an option for submitted files to be confidential. Opening old project files correctly has a high priority.

1 Like
15

Will do. Apologies for a maybe stupid question - Where did you find the “8.0.5.71” build?

16

KiCad main page - download - Windows - Testing builds.
https://downloads.kicad.org/kicad/windows/explore/8.0-testing
I use the x86_64-lite file

17

Ah, Thanks. I’m on Linux. I probably should have mentioned that…
I was looking at the Linux install page, at the Flatpaks, so I could install and test without disrupting my current install. There doesn’t seem to be any version info.

18

I installed from the Testing Ubuntu PPA, which gave me:
kicad_8.0.5-testing-180+202410031849~15582773bd~ubuntu24.04.1_amd64.deb
It looks like the references have worked, so that is good news.
Thanks again

1 Like
19

We don’t currently have a way to install testing builds with Flatpak, sorry. Looks like you found the PPA though.

1 Like
20

I made the same jump with a project with four sheets and a couple of hundred components two weeks ago. After i noticed that just “open the project and hope for the best” is not the ideal approach, i first upgraded the libraries and paths, and only after that opened the project itself. This made a major difference. If i remember correctly i had:

  1. one problem with a multi unit component (reference lost)
  2. moved and resized references on the silkscreen of all connector components
  3. numerous DRC errors on overlapping solder masks
  4. one F.cu track was mysteriously lost in thin air
  5. one footprint had an extra line on the user layer

All the errors could be corrected manually, and the whole process took me less than two hours. (Solve (3) by: manually ticking “Allow bridged solder mask apertures between pads” on most footprints).

I think this is remarkable achievement of the KiCad development team. :+1: :+1: :+1: