Best way to correct duplicate symbol references for PWR?

I have generated a schematic by cutting and pasting from another and duplicating the results. Everything looks to be properly “assigned” but when I click the “Fill in symbol designators” I get several messages for example "Error: Duplicate items #PWR7A ".
Looking at the GNDs with Edit I can see that these values are assigned but not displayed, and are, of course duplicated, with my copies. The obvious corrections are

  1. re-designate the whole schematic. This is not a good option as I want to keep the other designators as is
  2. go in “by hand” and change each ground. (that would take a lot of beer!)

Is there a better way to do this (or am I letting “prefect” get in the way of “good enough”)

Thanks-Fritz (364.8 KB)

Run an ERC-test. Ignore all warnings. After the ERC run the annotation-tool with “keep all existing annotations” set. Be happy.

Just seen: many wires and symbols are off-grid. That’s not recommended (at least not by me).

A bit curious to what’s it all about I did run the annotation and got 18 errors, so 9 duplicates:

I do not see how these few items equate to:

On a more general sense, I am not sure what your end goal is.

You have a hierarchical design and “Amplfiers1” seems to be identical to “Amplifiers2”, but they are different schematic sheets. One of the powerful features in KiCad is that you can use multiple instances of a hierarcical sub sheet.

OK and thanks. That worked–but it is a bit un-intuitive. I will add it to my notes

Paul–nothing special with the end goal–just 4 duplicates of the same driver circuit with different references on the parts of course. I think you are indicating a better way to do this–looking thru the manual I don’t see it.

(PS-manually updating all the grounds would take a long time–something I do in the late evening with a few beers)

When you create a hierarchical sheet symbol, it asks you for a file name.
In that box just enter the file name of an already existing sheet.
This surely is in the manual, but it’s such a small thing that it’s easy to overlook.

So in your case, use a very simple sheet with just one of the amplifiers, and make 4 copies of it.
I used Duplicate [Ctrl + D] from the popup menu in the example below. (100.7 KB)

A big advantage of this approach is that our sub circuits will also be the same.
It also enables working with the Replicate Layout action plugin in KiCad.
You may have to mentally adjust because you have less control over the Reference Designators, but that is a small price well worth paying in my opinion.

1 Like


I just noticed you put measuremts on a copper layer on your PCB.
That’s not a good idea. Put these on one of the user or fab layers.

Thanks Paul, you put a lot of work into this post. I see the hierarchical sheet material in the document–apparently you have to click help from the eeschema program (not the startup menu).
A lot to learn but the new KiCad has a lot of good things and works very well for my purposes.

I did not put much time in it. Maybe 10 minutes or so.
One you know how it works it’s quite easy.

It’s also nothing new, Hierarchical sheets were definately already in KiCad V5, and probably a few versions earlier.

Including multiple copies of the same sheet is described in the “complex hierarcy” section of:

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