Can you make parts of a schematic inactive?

Query. In coding programmers often place comments to add descriptive texts which are ignored by the computer

// iAmNothing();

Is there an equivalent in Kicad with which I can ‘comment’ out parts of the schematic without deleting or moving the content?

Those things on the right, is just some doodling. It is in alternative approach to solve some problem. Besides making a new project with a new schematic, is there a way where I can leave the doodle be, but let it be ignored by kicad. So no footprint relation to PCB, no annotation, no ERC error…

Right click menu gave me no clues.
I tried finding something in hotkeys list with some search phrases.
Dito with the manual. Couldn’t find it so quickly.

Kind regards :coffee:


I don’t think that currently is possible but i think that this could be an interesting and useful feature request.

Speculating on the feature behavior:
there could be a ‘graphical boxing’ feature to ignore stuff, boxing makes stuff inactive and light gray.
You delete the box, stuff returns active.

I’ve seen someone proposing similar kind of behavior to setup netclasses, maybe a common gui mechanism could be generalized…

There are many things to consider, reference values for one, I think the risk would not warrant the reward.

Perhaps similar functionality could be achieved with a separate stand alone Schematic sheet within the same project, Notepad.kicad_sch and open this in the Schematic Editor in standalone mode.

That’s for sure! i’m not even close to knowing the inner working or the architectural design of KC, i’m just a poor user :slight_smile: . A graphical driven feature could be very expensive or even impossible to do, the only thing i can tell is that the idea is interesting, implemented in a way or another i could make use of it.

Perhaps similar functionality could be achieved with a separate stand alone Schematic sheet within the same project

This sounds okay to me :smiley:

I did find one thing in some-not-my schematic. Something similars seem to exist allready. A symbol seems to have a checkbox named ‘do not populate’. it greys out the symbol and adds a big red X

If I could toggle this box with a hotkey of all selected items at once. I’d be happy too.

That would not be that hard to accomplish, would it?


That is coming in V8 . . . but that still puts the footprint on the PCB just doesn’t populate the footprint with the component. Perhaps you also want “Exclude from board” ?

Haven’t you seen this:

It was not long ago (yesterday) and looks like an almost identical problem.

I think I do :smiley: So recommended I try out the release canditate of K8?

By all means have a play . . . but don’t forget if you save a file in V8 you can’t then open it in V7 . . . make sure you have good backups of anything you cannot afford to lose.

In addition to the link @Piotr posted, you can do this (video)…
Has individual Text items and a Text-Box
(did not do in video but, you can have no background color - I was just tinkering…)

Being able to turn off elements in schematics for simulation is a very useful feature when available, this is something you can do with QUCS, great for turning on appropriate sources for different simulation types for example

oh you mean to remove values and production info to ‘clean’ the schematic for confidential purposes ?

Note that “Exclude from simulation” is already an attribute that any symbol can have. In v8 the properties manager will make it slightly easier to set on multiple symbols, in the same way that the do not populate and Exclude from board attributes can be set.

1 Like

Yes, put a # in front of the component name i.e. #R34

Not up to date.

No. That is an ancient left over from an age where this was used to mark power symbols. In KiCad V7 you can set fabrication attributes in the properties of a schematic symbol.

1 Like

I’ve done it successfully for documentation purposes, like in the attachment. All the symbols in the cyan box are real symbols, but I’ve checked their “Exclude from bill of materials” and “Exclude from board” box, and given them a ref designator prefix that won’t clash with anything, even if I reset designators.

For the more general task of “commenting out circuitry”, I can see the benefit for sure but personally I don’t mind applying a similar philosophy as I do to code comments:

  1. if it’s temporary, then just leave it there - it wont hurt anything until it will, and then you’ll get a warning
  2. if it’s to disable something, then do the work to make it innocuous (eg. move to separate sheet or set up a variant or something, sort of like an #ifdef equivalent)
  3. if it’s something you don’t want any more, then just delete it and rely on your version control if you want it back (ie. no “dead code”)
  4. if it’s for documentation, do as I suggested above.
1 Like