How to see all the same net in a schematic

I am new to KiCad having been using Eagle for far too long. One of the Eagle features I find very convenient is that I can click on a net and all the same nets in the schematic highlight.

I am trying to copy an Eagle schematic exactly. The schematic has three discreet PCB’s so I need to label power and ground different for each PCB. In my Eagle schematic I have +5V, +5V-2, and +5V-3. In the KiCad symbol editor, I did a right click to select 'New Symbol", gave it a name of +5V-2, and selected “Derive from existing symbol” +5V. However, when I put the new symbol +5V-2 into the schematic and connect it, the name is still +5V. How do I make the +5V-2 unique? And how can I look at all the instances of a net on a schematic?

Use toolbar at the right border, second tool from top. The tooltip therefore is “Highlight wires and pins of a net”.

What do you mean with this:

KiCad can directly open Eagle projects and convert them to Kicad. Both schematic and PCB. Just do: KiCad Project Manager / File / Import non-Kicad Project / Eagle Project

Don’t derive the power symbol it doesn’t do what you think. Inheritance is for things like 74LS00 → 74HC00. Look at the innards of the +5V symbol then make a new symbol +5V-2 to have the same properties except for the symbol and (single) pin names. And you need to save it in your own library of course, you shouldn’t modify the system library.

Edit: Also remember in KiCad 1 project = 1 board.

PS: Is a discreet PCB one that doesn’t gossip? :wink:

Eagle show-command: like @janvi said: it’s “highlight net”-command from the right toolbar. Additional: the kicad user-interface is very hotkey-centric. So look into the Preferences–>hotkey–>schematic section. If you type “highl” into the search-field you get all hotkey-comands connected with highlighting actions. My advice: try the “highlight net under cursor” first.

additional +5V-power symbols: This is comparable to eagle. steps:

  • copy the original +5V-symbol into your own library (don’t use derived symbol!)
  • in library-editor: rename the copy to +5V-2
  • in library-editor: rename the PIN of the symbol also to +5V-2 (Pin-name == symbol-name)
  • correct also the symbol-description string
  • save symbol, now it’s ready to use
  • at first use make a check: draw a little wire-segment onto this power-symbol, click to select this wire-segment and look onto the statusbar: is the shown net-name == power-symbol name?
  • look into kicad schematic documentation, there are two extra sections for power-symbols: (Schematic Editor | 6.0 | English | Documentation | KiCad) and (Schematic Editor | 6.0 | English | Documentation | KiCad)

redraw eagle schematic: I understand and second your approach (as opposed to using the eagle importer):

  • no importer is 100% reliable
  • more important: you don’t know directly, which part was correctly imported and which part not - so you end up with a schematic/board which might include errors, but you don’t know how many and were to look
  • last point: redrawing older projects is the best way to learn a new CAD-tool. You already know the destoination and can concentrate on the workflow. Additionally it’s the best time to add little improvements/bugfixes into the schematic.

Edit: Also remember in KiCad 1 project = 1 board.

With the latest changes in the v6.0.10 branch and v7 this restriction is somewhat loosened. The current situation is similar to eagle:

  • you can create multiple board-outlines in the board editor
  • you can place the footprints + do layout on these different boards
  • if you place same signal tracks on different boards you will get ratsnest-lines which connect these boards, you have to live with these (ignore them)
  • all output files include all of the boards together (gerber, 3D-step, pnp-files).
  • So the pcb-fab-house has to deal with separating the multiple boards

With eagle this approach (pseudo-multi-board) worked well enough for me. I made a little test in Kicad some days ago and it seems now to work also. I have an upcoming multi-board project (maybe, contract currently not signed), so I can tell in 4…6 month if it also works in Kicad (for a real project).

It was told but I will say once more.
The key is to rename not only the symbol but also the PIN name.
At schematic you see the symbol name while net is defined by pin name.

Imagine TTL IC and you want to have hidden VCC and GND pins. The pin name have to decide the net and not the symbol name (history…)

Does the 3D viewer work with multiple outlines now? It used to throw a fit it there wasn’t a single closed outline, so even a V-cut on the EdgeCuts layer would block rendering.

Does the 3D viewer work with multiple outlines now?

Yes. but all outlines must be closed. Cutout in every board also works (must also be closed). So simple V-cut line on edge.cuts layer don’t works.
example project (v7-file-format): (24.0 KB)
notice the remaining ratsnest-lines between the two separated boards - thats currently the price to pay for this “multi-board” solution.

3D-viewer and 3D step export works (again: you get all boards in one file/image. So for 3D-mechanics you have to separate them in the 3D-Cad - but theres my knowledge ~0)

Interesting, so the closed boundary algorithm in the viewer doesn’t regard a shared edge as a boundary or try to remove it for the purpose of rendering.

Thanks all for the information. I have made the power symbols work. And know how to highlight the nets.

I did import the Eagle files into KiCad, but want to do the circuit from scratch just to learn.