Importing Eagle to Kicad fails

Software
1

First time posting. I appologize in advance for whats probably been discussed 1000 times already, but I cant find the answer Im looking for.

I have an older Eagle project I would like to import. Specifially I have schematic file and a board-file. Thats it.

I can import and open both schematic and board in Kicad 9.0.5. Apart from a few small errors it looks good at first glance. Problem is that I cant get the schematic and layout to sync correctly. When I try to update the layout from schematic (F8) Ii get an error for each component like this: .Error: Cannot update R69 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).

I can sort of understand that the footprint is not a standard Kicad footprint and therefore not present in any of the standard-libraries, but the footprint IS correctly shown on the layout so I assume its a problem linking the information somehow.

Any ideas on where to start? I could assign new footprints to all components, but I expect that I would then alos have to place each component again, and I would really like not to.

Kind regards

2

Import the whole project (from the project manager).

If you import the schematic and the PCB separately, you do indeed loose the connection. This can be repaired but that needs some (careful) extra work.

3

And update to V9.0.6, your version has some annoying bugs

4

I cant figure out how to import anything else than just the board and schematic. The import-function looks for files with .sch and .brd extensions, so based on that it dosnt need a “project-file” or anything else.

The eagle-files are my own design and there is a non-zero chance that I did something wrong on those :slight_smile: (I had PCB´s produced based on the eagle-files and those worked fine, - so the design is not totally corrupt)

Kind regards Troels

5

From the KiCad project Manager: File / Import Non-KiCad Project / Eagle Project and then select the eagle schematic. KiCad will then do the PCB too.

6

Hi Paul.

I think, thats exactly what Im doing.

This is working:

  1. Schematic is loaded and shown almost correct (minor corrections)
  2. Layout is loaded and is linked to schematic ( selected parts in layout is highlighted in schematic and the other way around.

This is not working:

  • When I try to update layout from schematic it works partially. A lot of components fail with this message:
    • Error: Cannot add R12 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).
      Error: Cannot add R11 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).
      Error: Cannot add R77 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).
      Error: Cannot add R10 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).
      Error: Cannot add R78 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).
      Error: Cannot add R9 (footprint ‘LLC-ATX-100x100 newTX-35:R1206W’ not found).

Some of the components that fail to add are modified/designed by me, but some of my components load just fine.

I did not setup any special paths for libraries, symbols or footprint.

Any ideas?

Kind regards Troels

7

This is pretty much everything you can expect from the importer. After a project is imported in KiCad (V6 or newer) then all used symbols and footprints are embedded in the project itself. After that further processing can be done by fiddling a bit around with library management. Library management in KiCad is not very difficult, but it can be confusing and you have to get the details right.

KiCad can directly use eagle libraries as far as I know, so that is one way you can progress further.

Another method is:

  1. PCB Editor / File / Export / Footprints to new library (And update the links).
  2. PCB Editor / Tools / Update Schematic from PCB (This is the other way around as the normal workflow. Main goal here is to get the footprint library links into the schematic symbols.)
  3. Schematic Editor / File / Export symbols to new library

If you’ve done these steps correctly then you have created a footprint and symbol library for your project, and further edits will use these libraries. Personally I prefer to go a bit further, and replace most simple parts such as resistors, capacitors and power symbols with KiCad’s native versions.

8

Hi Paul

Thank you for the assistance. It makes sense to export from the project to new lib´s and use those. - but Im supprised that Kicad dosnt do this as default?

I could really use a few pointers as to how the new lib´s are added to the project.

Troels

9

Library management is explained both in KiCad’s manuals, FAQ articles here on this forum and in various other places.

The importer is just an importer. Personally I prefer the manual approach: KiCad has relatively simple tools to do simple things, and you string them together in the order you want. If you want to go further with automation, you also have to make the tools more complicated.

10

Hi Troels,

I have imported many eagle projects to KiCad and have successfully brought them to manufacture, assembly and function. So, I completely understand your struggle.

image
image617×538 32.3 KB

FYI, I have and had KiCad 9.0.2 installed.

After following the image, I always choose pcb file of eagle (.brd) when importing. After choosing your brd file, you are asked to select a folder for your imported project (kicad) to be saved in.

Then you must see the window “Edit mapping of imported Layers”. I always do this:
I first do “Auto-Match Layers” and then I match every layer that is left to a user layer. Because as far as I know, once importing is done, you have no longer the chance to retrieve any missing layer. Yes, you can import again. But definitely you’ll lose your edits.
I then take screenshots or notes that which layers are connected to which user layers, then if later needed, I activate the required user layer. In this way I never lose/miss layers again.

Here comes the important part: You have to save both imported schematic and imported pcb. My suggestion is to first save and then close everything and open them again.
Then hit Switch to PCB Editor in schematics, and vice-versa in PCB to make sure they are bonded with each other.

Also, in order to see the library that kicad has converted from eagle for you: from project manager, go to footprint editor, a library, sharing same name with your project, consisting all converted footprints, must exist there.
Or
simply go to PCB, select one footprint, open its properties (hit E or double click), then “Edit Footprint…”, then on the upper part of the window you see a yellow bar, click on the blue linked-like text “Open in library {your_project_name}”, when you click on that, you open the footprint in the library imported from your eagle project. On the left side you can see your other footprints.

I hope these could solve your issue.

Mahsa

11

That is very likely completely irrelevant. KiCad imports both the schematic and the PCB via the Import Non-KiCad Project … function.

That is good advise. KiCad does have some quircks (and latent bugs) and some settings only properly propagate after a restart of KiCad.

I think that you’re right here: That KiCad should create project specific libraries for the project automatically. If that is so, then you can skip the method I mentioned earlier, as it is (almost) a duplicate of what KiCad did during project import. (but you can always do it later if you wish so).

12

Yeah, you’re absolutely right . It is probably something more feelings related. Maybe once I had schematic selected and I got bad results therefore now I get bad feelings :slight_smile: