How to update ratsnest after modifying reference designator number of a component

Hi, I’m trying to change the reference desginator numbers on some existing components which I have placed on a PCB layout. I am doing so by right clicking on the component and selecting ‘properties’ and then changing the field labelled ‘reference’ in the table. when I exit the properties page I can see that the reference designator displayed next to the component has changed accordingly but the ratsnest does not change… even though it should now show a different connection to before.

does anybody know what I’m doing wrong please?

I’m using Kicad version 5.1.12

Many thanks

ok I’ve worked it out…

  1. modify the reference designator for the component you wish to change
  2. ensure ratsnest is switched on (so that you can see when it changes the connection)
  3. go to tools menu and select: load ratsnest…
  4. make sure ‘reassociate footprints by reference’ is enabled
  5. click update PCB to finish

The ratsnest is now updated.

It seems well simple now that I’ve worked it out but I thought I’d post it on here so as to help anybody who might be struggling with the same issue.

1 Like

The RefDes is just some text string.
Internally KiCad uses UUID’s to identify schemematic symbols, footprints, and the links between them.

In your step 4). when you select Reassociate Footprints by Reference you instruct KiCad to use the RefDes instead of the UUID’s to do the matching between the schematic (which is master of the netlist) and the Footprints on the PCB.

Thanks Paul,
So is the way that I’m doing it the most efficient or is there another method which is better?

Are there consequences to not using UUID’s?

I do not understand the question.

KiCad always uses UUID’s, It’s just not possible to not use them, even if you do not see them.

Just for clarity:
KiCad does not synchronize automatically between the schematic and the PCB. Either via: Schematic Editor / Tools / Update PCB from Schematic [F8] or the other way around from the PCB Editor.

(There are some more slightly oscure methods, such as exporting a footprint Association file from the PCB Editor, but those are a bit outside of the normal workflow).

1 Like

symbols in the schematic get UUIDs which are sort of like unique timestamps, when they are created/added
they also must have Refs (RefDes) but these don’t mean much before they are annotated, and they still don’t mean too much because they can get re-annotated differently afterwards

the question here is how do you decide which “symbol” or “component” from the schematic maps to which footprint on the board:
kicad has always (at least since v4) allowed (at least) two ways to do that - by RefDes or by timestamp (UUID)
there’s no right and wrong in general, they behave differently, thus each of those can be right or wrong depending on the situation, that’s why the choice is left to the user

if you have an existing, routed board, and the RefDes are chaotic, you can completely re-annotate the components - in this scenario you want to map them by UUID

mapping by RefDes is (or at least used to be) useful in other scenarios like this one: Tip: Schematic: move/cut/paste things to a different place without ruining the PCB (Kicad5) (notice how this technique relies on both kinds of mapping)

which of the two is right for you is hard to tell before we know the bigger picture of the situation and the final goal
it’s definately a good idea to be aware of these kicad internal mechanics to be able to decide yourself which thing to use or predict the potential consequences of your manouvers

1 Like

Thank you both for these answers.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.