Isolated power nets in hierarchical schematics?



I have a design that has 12 separately-isolated input signal conditioners. This involves creating galvanic isolation of each of the input conditioners from all of the others and from the main processor. I will accomplish this with 12 isolated power supplies, one for each isolated signal conditioners.

I am having trouble drawing the schematic in EEschema. Since all signal conditioners are the same, I want to create a single sheet for the conditioner design and refer to it from each of the conditioner instance sheets. However, this means that the power nets are connected together.

Is there any way to name a net with the name as given on the conditioner-design sheet to which an instance number is automatically appended? My only alternative to this is to name no nets and use no power nets (no power symbols or ground symbols) on the conditioner-design sheet. This makes the sheet very hard to read.

Suggestions, please?

Thank you,



Use hierarchical pins or local lables inside of hierarchical sheets. Both of these will be uniquely named automatically no matter how often you instantiate the sheet. (They are prefixed with the full sheet path)


Eh yes, afaik the power symbols under the hood are ‘just’ global labels, so you won’t get them to behave the way you want.
@Rene_Poschl gave you all the options there are in KiCAD.


I get it that I need to use either hierarchical pins or local labels. My issue is that I am using one sheet of the design (the “proto” sheet) as the input file that gets instantiated 12 times. I also get that the power nets on each of the instantiated sheets will be connected to all of the others unless I use only local nets on the “proto” sheet. And I get that I don’t have to explicitly connect the local power to each device in the "proto"sheet to have them connected internal to each instance but not between instances.

However, I have 12 instances of 150+ parts each, and the instances have to be identical, so I need to use the “proto” sheet idea. With the large number of parts, I have a large number of power and ground connections. When I use the net-name approach, it works, of course, but it clutters up the sheet and is not obvious to others. Is there no way to define a symbol that at a glance indicates a local power net? I can’t believe that this isn’t possible in some CAD tools, and it would be very useful in KiCad, especially as the tool is becoming more mainstream all the time.

All this would really need is a 1-pin symbol that could be defined by the designer and that:

  1. would be annotated with a part number automatically,
  2. conveyed the properties of a local net name, or even applied a non-visible net name, and
  3. could have a power flag attached.

Best regards,



Right now there is no way to define a non global label via a symbol. To be honest the power symbols are a hack right now and will most likely change with the new file format that is expected with version 6 (Version 6 is to be expected in two years time at the earliest)

You can however look over at the bugtracker if there is already a wishlist bug open for your request. If there is than add your voice to it, if there is not then create a new bug report for this feature.

However until this is implemented you really only have the option to use some kind of local label for this task (local label or hierarchical pin depending if the potential should connect to the outside in any capacity or if it is completely local)


I think it might work if you draw the isolated SMPS circuit on a hierarchical sheet, and then use local labels for the power on the isolated part of the SMPS.

But I’m not sure unfortunately.
I think I tried to get this to work in KiCad V4 quite some time ago, but I abandoned the idea before it was finished.


Thanks to you both.

Paul, I have a SMPS for each of my instances, and since it was drawn on the “proto” sheet I instantiate one on each sheet, which is what I want. The local labels work fine on the sheet and they do the job. The problem is that they make the sheet very hard to troubleshoot as they have no visual impact in the way that a power or ground symbol does.

I suppose that I could create a “component” that had one pin and a net name, and maybe some text that said “local power” in large letters. I will try that now.

Rene, your input is valuable, thank you bad news that saves time searching is much better than no news at all…

Thanks again to you both.

Best regards,



My first attempt at something like this would be to start with the PWR_FLAG symbol, change the glyph to what you want and convert the pin type to “Power Input”. You will still need to use PWR_FLAG symbols to mark the “source” of the power, and the net your symbol connects to won’t inherit the pin name for the net name (like how power symbols work) so you will still want to use a local label near this symbol. But that should give you the graphical functionality you want. Note, you may want to somehow indicate that it is a local power connection (maybe the symbol’s value set to “local” or something like that).


I am not so sure it is a good idea to bodge something just to get the graphics of power symbols. Readers of your schematic might not know about your bodge and be confused.
You might forget about it years down the line. You might accidentally place a real power symbol and screw your whole project.
You might forget to place the local label (kicad might not complain as there are two pins on the same net and it is therefore not unconnected. Depends a bit on the combination of pin types.) I would consider this error mode as most frightening. (Your bodge disables or hinders ERC.)


Thanks Rene, your thoughts are much appreciated. If I did it, there would be accompanying text attached to the graphic that said “LOCAL” in big letters, but that doesn’t solve the need for a net name, I agree.

another option KiCad development folks might consider is having a net name that has enlarged text and a graphic that has a power-like symbol. That would do what I want.

Best regards,



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