I have been making bulk updates via the Symbol Fields Table, which is a fantastic tool. However, when I close the table and go back to the Schematic Editor, all of the newly-updated symbol fields are visible, “polluting” the schematic to the point of it being unreadable. I have spent some time trying to find a ‘select all’ option for these custom fields in order to switch them off. I’ve poured over the Kicad user guides to no avail, but I may have missed something.
Does anyone know how to bulk toggle-off these fields?
As far as I know there is no option to bulk toggle off specificly only these fields.
You may try the Edit–>Edit Text&graphics Properties dialog (picture). But this sets all symbol fields to “not visible”
It may also help to set the selection filter (only visible if hierarchie panel is visible) to “only text”. This helps in selecting the new added fields. With “Delete” key you set all these selected fields to “not visible”.
I believe this is a regression from KiCAD 8’s default behaviour. In KiCAD 9, if you add a field from the “Symbol Fields Table” the default is to automatically show in schematic. However, if you add a new field through the “Field Template” or on the individual symbol property, the default is to not show in schematic.
This seems inconsistent in the design and different from KiCAD 8. In large designs it’s very inconvenient to manually make each field invisible once you’ve used the bulk update feature using the “Symbol Fields Table”
I’m not seeing this is ‘fixed’. At least not in 9.0.2 RC1 on Windows10. In anticipation of migrating to V9, I wrote (mostly Grok) a python program to parse through all of my schematic symbols and add a new field named ‘Description2’. I did this as in a past major version upgrade requiring migration of user libraries, I believe one of those past migrations overwrote the edits I had made the ‘Description’ field so I figured I could prevent that in the future by creating a new field that wasn’t already a default Kicad field name.
Anyway when I update my ‘symbols from library’ in my older schematics with my library symbols that now has this new field, this new field updates with it visible on all my parts even though the field is set to hide in the symbols themselves. If I just place a symbol from my library that has the new field, the visibility setting in the symbol is honored.
Fortunately as mentioned above, there’s an easy workaround using the bulk edit functionality. I’m embarrassed to say how much time I spent setting them individually. I even briefly looked in the native S-parameter file and found where I could have Grok and I write a python program to ‘fix’ it. Then it dawned on me to look at bulk edit more…
Oh yeah, you CAN apply bulk edit changes to only a specific field. See attached:
The issue with showing symbol fields after using the “Update symbol” command was a different one. That was fixed in the last 2…3 days, the most recent testing build already incorporates the fix (just checked).
Also nice find with the “Filter by field name” option in the picture above, I had overlooked this for a long time.
Ahh, if it was fixed in the last 2-3 days, it would make sense that I didn’t see it in 9.0.2 RC1 as that was posted a week ago. I’m brave enough to run RCs, but not so much nightlies. I’ll keep my one good eye out for it when either the next RC is posted or 9.0.2 formal. Thanks!
We are talking about bugfix branch, not about development nightlies. It’s very unlikely that you would get a new problem with daily testing builds, and even then you can go back to latest working version. The announced RC for the stable branch is just another testing build, nothing special. Actually even the final bugfix release is just one testing build!
Thanks for the heads-up, but with the functionality of being able to do bulk edits on specific fields, this ‘issue’ is easily resolved with a few more button clicks. I’m in the middle of doing my 1st complete design with V9 so I plan to stick with 9.0.2 RC until either I finish and tape out or an new ‘release’ build comes out.
