Mapping 3D models in design imported from Eagle

Dear all

I‘m rather new to KiCAD and I‘m very impressed with the Eagle CAD import converter which I‘m using to inspect the 3D view missing in older Eagle versions.

One question (actually, two questions): I‘m able to map individual footprints to 3D models, but I‘ve to do this for every single instance of an element. Is there any shortcut to map all instances of an element to a model at once? Is it possible to save the mapping in a file so that I can reuse that whenever I reimport the Eagle design in KiCAD?

Thanks for any suggestions!

Best regards,


The way to do this is to create your own library of components, and then make sure your components use that library.

  1. Hover over a Footprint in Pcbnew and press E for edit.
  2. From the Footprint Properties window: image
  3. This opens the footprint in the Footprint Editor
  4. Footprint Editor / File / New Library / …
  5. In Select Library Table choose Project to make it a project specific library.
  6. Save your Footprint in your custom library.
  7. Add more Footprints to your newly created library in a similar way.

Just to be sure, verify you own library is in the library table:
Pcbnew / Preferences / Manage Footprint Libraries / Project Specific Libraries

In the Footprint Editor you can also click Tools / Load Footprint from PCB

And when you have one of each footprints in your library you can:
Pcbnew / Tools / Update Footprints from Library

Oops, this updating may not work.

The next best step is most likely to go back to the Eeschema.
In Eeschema you can modify the Symbol to Footprint mapping so all schematic symbols use the footprints from your newly created library.

Eeschema / Tools / Edit Symbol Fields*
Then, in the Footprint column of the spreadsheet, click on the book case. image Then browse to your own library and select the right footprint from that library by double clicking on the text of the library Footprint name.

Now, still in the “Symbol fields” spreadsheet you can copy and paste the Footprint library reference to other components with the same footprint.

In the Symbol Fields spreadsheet there are options for grouping (schematic) symbols in different ways. Experiment with the checkboxes and watch how the spreadsheet changes. With grouping you can speed up the copy & paste operations.

If you’ve changed some of the references, close the Symbol Fields spreadsheet with the big button: image and then [OK].

Back in Eeschema / Tools / Update PCB from Schematic to syncronise the Footprint reference changes you made in the schematic with the PCB.

I did this with KiCad open, but without actually doing the whole process. I may have missed some small steps, but this short walk-through should give you an idea of how to do it.

There may be shortcuts. I seem to remember that KiCad can directly work with (or convert) Eagle libraries, but I have no experience with that.

For additional help, you can of course press Help on the right side of each of KiCad’s sub programs. The FAQ here on this forum is the most up to date source of information:
In the FAQ, pay special attention to the entries concerning library management.

Or, click on the magnifying glass in the upper right corner of this forum for searching the forum.

Hi Paul

Thanks for the detailed guide. In fact, it already helps to map the footprints in the library auto-generated by the Eagle import. What I did wrong initially was that I mapped the 3D models by opening the footprint from PCBnew, which only changed that specific instance. Doing the same by opening the auto-generated library in the footprint editor changed the models project-wide. I should be able to proceed from here.

Thank you very much again for the quick and helpful response.

Best regards,


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.