I’m cleaning up a schematic, originally created in Eagle 9.6 which has been imported into KiCad 8.0.3. I used Tools/Edit Symbol Library Links to update from project-specific libraries (created on import) to KiCad standard libraries.
Looking at the resistors, I notice two things:
The orientation is off by 90 degrees. I looked for a way to select all resistors so I could change the orientation, but didn’t find one.
The resistor values are not displayed and once they are, individual values like 68k1 have been replaced by a constant string “R-EU_R0805W”
My questions:
a) Did I miss an option on import, or do something wrong when updating symbol library links, that caused this?
b) If not, is there a way to select all components that match some pattern and operate on them as a group or do I just settle down to rotating them all, one by one?
I have not seen this before. I have seen that KiCad’s resistors are a bit smaller, and thus you have to reconnect the wires, but that is a different issue.
In this other thread:
you mentioned a github link to “ondesModulaire” and I wanted to have a look at it to see how good eagle imports are at the moment, but I got a bit lost in all the different sub projects and many posted files.
Maybe eagle has different (official) ways of specifying part values. If so, then making a bug report for this may be a good idea.
There is no requirement to do “update symbol library links” and switch from Eagle resistors to KiCad resistors. As you have seen, they are oriented differently, so if you do this step you will have a lot of cleanup to do. I would just skip this process and stick with the existing Eagle imported symbols.
There is nothing wrong with sticking with project-specific libraries containing symbols imported from Eagle. You can also copy or move the imported symbols into new custom global libraries, and then update library links to point to these (for example, to share the imported Eagle symbols between multiple imported projects)
That GitHub repo is about a series of Eurorack modules, and is basically my own working notes to collect my thoughts and to record what I have done. For someone wanting to build or modify a module, it is easiest to read the markdown files which link a lot of images, schematics and so on.
For your purposes though, you don’t need all that and just want some sample Eagle files. So I have just now collected the Eagle-specific files into Eagle directories; have a look at:
I just confirmed that creating a new KiCad project, editing the blank schematic, and importing an Eagle 9.6 schematic looses the values (for all parts, not just resistors). The name and the value become identical on import.
If not, is there a way to select all components that match some pattern and operate on them as a group or do I just settle down to rotating them all, one by one?
As this part of your question is still open: there are multiple ways to do such a multi-selection:
use the “Edit symbol fields” table (from mainmenu–>tools). On the top this dialog has a field for a filter string. You could also sort by every column (value/symbol/footprint/…).
Use the search panel from mainmenu–>View-_>Show search panel. This dialog also exhibits a filter field.
Both dialogs could select multiple symbols (selecting with Shift/Ctrl + mouseclick). There is however one important restriction: the selection works only for items on the same schematic page. Selecting symbols from different pages and modify them simultaneously will not work!
The “symbol fields table” has a handy checkbox to restrict the shown symbols to the current page, to prevent accidental selection across multiple pages.
After the selection the properties panel is a good way to change the symbol angle for all selected symbols at once.
