Net connector symbol

I am switching from the venerable Designworks to Kicad. In general, Kicad is superior, but there are a number of features in Designworks that I miss. A big one is the “Net connector” symbol. In Designworks, I can add this symbol to any net, and it creates a link with all other symbols, and displays the net name and the page and grid location(s) of the other connectors. Example:


I find this to be a very useful feature. I don’t particularly like the “connect by name” method, because on a multi-page schematic, it can be very difficult to see all of connected nets.

Is there an equivalent function in Kicad? Or, can this be added as a feature request?

I have never used Designworks. How does that know which nets to connect if it does not use the “connect by name” method?

KiCad does not list other places a label is used, but you can export a netlist with: Schematic Editor / File / Export / Netlist. KiCad’s native netlist format (you can also export other formats) looks like:

      (node (ref "U4") (pin "9") (pinfunction "Vdd_a") (pintype "power_in")))
    (net (code "2") (name "+5V")
      (node (ref "C53") (pin "1") (pintype "passive"))
      (node (ref "C54") (pin "1") (pintype "passive"))
      (node (ref "C55") (pin "1") (pintype "passive"))
      (node (ref "C56") (pin "1") (pintype "passive"))
      (node (ref "C57") (pin "1") (pintype "passive"))
      (node (ref "Cut485") (pin "1") (pintype "passive"))
      (node (ref "D1") (pin "1") (pinfunction "K") (pintype "passive"))
      (node (ref "D51") (pin "1") (pinfunction "K") (pintype "passive"))
      (node (ref "L50") (pin "2") (pinfunction "2") (pintype "input"))
      (node (ref "NT50") (pin "1") (pinfunction "1") (pintype "passive"))
      (node (ref "P3") (pin "33") (pinfunction "P33") (pintype "passive"))
      (node (ref "P3") (pin "34") (pinfunction "P34") (pintype "passive"))
      (node (ref "U33") (pin "3") (pinfunction "VI") (pintype "power_in")))
    (net (code "3") (name "+24V")
      (node (ref "C24") (pin "1") (pintype "passive"))
      (node (ref "C25") (pin "1") (pintype "passive"))
      (node (ref "C26") (pin "1") (pintype "passive"))
      (node (ref "C27") (pin "1") (pintype "passive"))
      (node (ref "D24") (pin "1") (pinfunction "K") (pintype "passive"))
      (node (ref "P3") (pin "35") (pinfunction "P35") (pintype "passive"))
      (node (ref "P3") (pin "36") (pinfunction "P36") (pintype "passive"))
      (node (ref "R24") (pin "1") (pintype "passive"))
      (node (ref "U50") (pin "2") (pinfunction "Vin") (pintype "power_in")))
    (net (code "4") (name "/485A")
      (node (ref "D485") (pin "1") (pinfunction "A1") (pintype "passive"))
      (node (ref "F485") (pin "1") (pintype "passive"))
      (node (ref "U485") (pin "6") (pinfunction "A") (pintype "bidirectional"))
      (node (ref "U486") (pin "6") (pinfunction "A") (pintype "bidirectional")))
    (net (code "5") (name "/485B")
      (node (ref "D486") (pin "1") (pinfunction "A1") (pintype "passive"))
      (node (ref "F486") (pin "1") (pintype "passive"))
      (node (ref "U485") (pin "7") (pinfunction "B") (pintype "bidirectional"))
      (node (ref "U486") (pin "7") (pinfunction "B") (pintype "bidirectional")))

This gives you an instant overview of all pins in any net, but you have to navigate to it yourself.

Or you just just the text find function [Ctrl + F] to find your label text. it cycles though all uses of the text over different schematic sheets, and highlights the text at the same time.

Does Designworks always show the locations a label is used? That does not seem very usable to me. Sure, you have a quicker overview of where it’s used, but the side effect is that labels take up much more space on the schematic. How can you for example connect a bunch of labels to a row of pins with that? It leaves only room for one line of text for each label.


The Net Connector symbol is assigned a name, and gives that name to each signal line it is attached to.

As for the clutter - this feature is mostly useful once the schematic has been turned into a PDF or paper document, which is pretty much the destiny of all designs. If the CAD system is available, then it’s certainly easy to highlight connected signals. But, in my experience, the lifetime of a design usually exceeds that of the system it was designed on by many years, so having a printed copy be easy to understand is very helpful.

I was just given a design to reverse-engineer, and I spent a lot of time looking for where signals were connected, because they used the “connected by signal name” convention.

I think they share some of the same functionality, but the big win for Designwork’s Net Connector is the list of other locations where a particular signal is connected.

Imagine a (printed) 10-sheet schematic, where a particular signal may appear on 6 of the sheets (say it’s “/Reset”). Sure is nice to be able to look at any instance of the /Reset connector and get a list of all the other sheets and coordinates where it appears.

In Designworks, signals had to be connected this way (or explicitly, with lines or busses). In Kicad, since the system has inherent “connect by name” functionality, this type of connector would be optional, and only used if there was a signal that appeared on my disparate pages.


global labels display the sheet numbers, where the same net is found. On my projects, that happened automatically.


When you click on the sheet numbers, you can select the sheet to move there.


Unfortunately, this doesn’t work in a PDF schematic.

Wow, I saw this once and thought this was a bug (it behaved buggy/inconsistent).

The labels must be enabled in the schematic setup, section General–>Formatting.
See picture:


Thank you, that is good information.
Wish the grid coordinates were listed, but, it’s better than nothing.

There are too many different or slightly different, or almost different net labels in KiCad.

Thanks for the tip!

And what I saw earlier was actually a glitch, as only one label had it, and I couldn’t interact with the “Intersheet References” field. When I renamed the label, the field became “?”.

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