You need to update the 3d models. Download them directly from github.
The problem is that there are now correctly scaled 3d models. Therefore the footprints have been changed to have scaling 1,1,1.
Another problem is that footprints are downloaded directly from github without control by the user. Whereas symbols and 3d models are not updated at all. (This results in inconsistent libs for the users.)
I would suggest to switch to a local footprint lib setup where you use the footprint lib setup. Either by following the tutorial by @bobc:
Or by using the footprint lib downloader python script found in the kicad-library-utils repo.
The footprints on your old board now need updating. (Once a footprint is placed on a board, it is copied into the header of the pcb file. Changing it in the lib does not update the original pcb.)
Another option is to have the old 3d files somewhere and change KISYS3DMOD to point to them when you few a old project. (If you cloned the git repo simply checkout the correct tag/release)
right click on ANY footprint in your layout, choose ‘Edit Parameters’
then hit the [Change Footprint] button
in the new dialog under ‘Options’ select ‘Update all footprints on the board’ and then hit [Apply]
… in case that fails…
open EESchema, re-create the netlist (export)
then back to PCBnew and import the netlist again, select ‘Exchange Footprint’ option ‘Change’ instead of ‘Keep’
Often when the components are of incorrect size, the scaling issue is due to SI vs imperial units. That is, that the 1.0000 scaling should be divided by 2.54 (one inch is 2.54 cm): 1.0000 --> 0.3937007874…
The by far easiest fix is to install FreeCad and add a macro
which is designed to make life easier when working with footprints and 3D-components in KiCad. The macro is called “KiCad StepUp”, and adds a bunch of tools to FreeCad, including automatic rescaling and so forth. It also makes much better renders (photo realistic).
Image showing FreeCad with the StepUp tools to the right of the capacitor. You can import mod-files, pcb-files, etc and export to STEP and WRML (with automatic rescaling and color selection to different parts).
It is also easy to move components to make them fit the footprints. This is a pain in the ass in KiCad.