I want to freeze/write protect all reference names. There should be only one place where I can change them. There may be caps but not duplicates. “Automatic annotation” in a wrong place, is a problem.
I deleted a component from our board. Lets say J8. I had to change the PCB too, of course. Then the manufacturing wondered what am I talking about, there is a J8 on the board. There were no new parts on the board, so KiCad had shuffled reference names. I don’t like that, not at all.
you can’t freeze/write-protect RefDes and care and attention to the annotate button must be observed.
Re-refdes’ing at the wrong point in a project is a disaster but also having the ability to re-refdes is a key concept and thus you as the designer has to take responsibility .
There are two settings you can use to help.
First, make sure Schematic Editor / Tools / Annotate Schematics / Options is set to Keep existing annotations. The other is to turn off the checkbox in: Schematic Editor / Preferences / Preferences / Schematic Editor / Annotation Options / [ ] Automatically annotate symbols
Another Idea: You can leave the automatic annotation on, but give it a prefix of Sheet Number X 1000
This way, you can see easily that the RefDes with those big numbers need some manual attention.
You can also limit the scope to the selection only, I just verified this does not annotate anything when there is no selection active.
Duplicates get caught by ERC:
And you can use: Schematic Editor / tools / Edit Symbol Fields for an overview of your RefDes and see if there are gaps or whatever. Click on one of the column headers to sort the table by that column.
But mostly, I agree with Naib. Annotating the RefDes is an quite important part of schematic design. Don’t click on random things nor let the cat walk over your keyboard. For emergencies, always have a working backup strategy in place.
Related to re-annotation… IMHO it would be very useful to have an schematic component “lock” attribute… just as there is a ‘lock’ attribute for components placed on a PCB.
On the PCB ‘lock’ means lock the location so it can’t be moved without extra acknowledgement.
A ‘lock’ attribute on the schematic would mean ‘lock the designator’.
Many times I’ve added components to a design and those components end up with numbers that don’t fit well into either the schematic or the PCB : just an OCD problem? Maybe not…
Sometimes you’ve had a service manual printed, so even if you have the wrong version manual, things like connectors should stay the same from rev1 to revN… except that when reorganising the schematic (parts moved around on a page, or between pages), a ‘re-annotate’ really makes a mess of things.
Connectors, jumpers, switches, tuning pots… no doubt more.
This is a good idea.
Connectors are key for this since there maybe a wiring schedule being produced in parallel. An updated refdes (and re-pinout) causes other assets to be updated.
As a design matures updating RefDes becomes more and more problematic
By the way, I can accept gaps in def res numbers. So new parts should get numbers at the end of list.
This is important. My problem was small, I just blamed KiCad. Note, not CAD but KiCad by name.
I think shuffling all RefDesignators is bad. Only exception is when a new component is added. And that should go to the end of list. Changing all of them is useless and harm full, but editing one is usefull. I think this means that when a new part is added, it gets its Reference Designator at the same time.
I wrote about this already, but I can’t see the post now. I wonder if I sent some private messages or something by accident?
Makes sense. Kinda always bugged me too but my projects are small and I tend to add them as I go, grouped in a logical order. 1xx (like power input circuit), 2xx (maybe a processor) … So, I guess more by block.
There is a gitlab feature request open demanding the immediate implementation of this feature: Request: Add reference designator (annotation) lock/unlock button. Useful for components on different sheets. (#15852) · Issues · KiCad / KiCad Source Code / kicad · GitLab.
Use the “Thumbs up” icon below the opening topic to increase the weight of that issue.
