Very quick fixes for ERC/DRC errors moving to v8

[retiredfeline]

Just upgraded to v8 on my workhorse and got it back to the way I want in a few minutes.

Restored my path variables by editing the vars variable inside kicad_common.json from the v7 version.

Restored my personal libraries by appending my library paths to sym-lib-table and fp-lib-table from the v7 version.

BTW, I edited the config files directly because I’m foolhardy or brave, depending on your point of view. I recommend you go through the GUI, especially if you are not familiar with JSON syntax.

Opened a v7 project and the checker presented me with hundreds of ERC messages about things off grid. Selected everything with Ctrl-A and from the context menu selected Align to Grid, and they were gone. The remaining handful of messages were about power symbols differing from library. Update symbols from library fixed those.

For the layout, the only important DRC message was also about a footprint discrepancy from the library. An update also fixed that. No errors for the parity check so hadn’t broken anything.

Back in business.

Don’t be scared if you get heaps of checker errors on upgrade. Usually there’s a simple fix.

[paulvdh]

Some small additions:

In the schematic, Align Elements to grid does sometimes create shorts. You can easily check for this by Updating the PCB from the schematic [F8], and then run a DRC to check for connectivity.

There is no real need to update symbols or footprints when they differ from the library. Especially in older and verified projects, updating to some newer and untested library may be a step backwards instead of forwards. Updating the PCB and running DRC in between steps is a quick and easy check if connections have changed.

If you want to keep the old symbols or footprints, then it is very easy to export the currently used symbols and footprints to project specific libraries. If you do this for footprints, then use PCB Editor / Tools / Update Schematic from PCB (reverse direction from normal workflow) to push the changed library references back to the schematic. The schematic always remains the main reference for “parts” in a project.