Component on schematic but not on PCB

If a component is part of the project, it should be on the schematic however, how is it represented if it is not part of the pcb layout?
For example, an LED is shown on the diagram but it is mounted via two wires to a panel.
The LED is not required for the pcb design as it wont be on the board (it will have two pads for the wires)
How do you get the LED ignored for the pcb view?

You can edit the properties of the symbol in question and enable the attribute Exclude from board.

1 Like

But exclude from the board will exclude the footprint needed for the 2 wires of the LED.

There’s no one right answer. You can add a LED symbol and exclude it from the board, while having separate connector symbol(s) for the soldering pads. Or you can use only a LED symbol and attach a footprint which represents the soldering pads; then you can allow Preferences → PCB Editor → Editing Options → Allow free pads, and move the pads independently on the board if you need to.

I typically handle off-board components by adding the appropriate connector to the schematic and then add descriptive labels. The pads on the PCB are labeled to match.
In this case it is a 1x2 header. If the actual pin header is not needed I remove it from the BOM before sending the files out for manufacture and assembly.

1 Like

The simplest is not to:

As you already realized (and pedro also mentioned) you need some kind of way to connect the LED to the PCB.

If you assign a THT LED footprint to your led, there is nothing preventing you from soldering wires to it, instead of the LED itself. A “complete / professional” way would be to add both a connector and a LED to the schematic, and then exclude the LED itself from the PCB. (The LED with wires and connector may even be some “sub assembly” on it’s own, including part numbers, drawings, etc. Although in a “high volume” production environment you would never want to mess with led’s bungling form wires. Those cost assembly time and thus money (imagine plugging 10 million connectors yourself just to add a led) For a production environment things like putting SMT leds on the PCB and using light pipes is more common).

A very simple and quick diy method is to assign some kind of connector footprint to the LED instead of a LED footprint.

1 Like

If I did this, I could then simply # the component? For example, D1 to #D1. This would prevent the LED being added to the PCB?

I would rather suggest to use “Exclude from board” attribute available in KiCad v6. The easy # thing was always a kind of hack. You can also exclude from BOM if you don’t want to show it in the BOM generated from the schematic.

That was the old method. Now you can choose to Exclude from board, and Exclude from BOM independently.

I am using an older version. I have looked at V6 however, as a novice, It blew my tiny mind.
I struggled to find library symbols on it for simple components like electrolytic caps. I was unable to make any use of it. (I concede that its my issue. Everyone else fill find it great)

There’s no considerable difference in this between v5.1 and 6.0. You will do a service to yourself if you give v6 another try, especially when v7 behind a corner and v5.1 will become more and more outdated. We can of course help if you are stuck on something specific. Getting Started in KiCad | 6.0 | English | Documentation | KiCad should be up to date for v6.

Same here.
If you’ve trouble with transitioning between software versions, I recommend you keep on using V5 you have now, and transition to KiCad V7 around March or April, after the first one or two bug fix releases have been made. By that time it should be quite stable and trouble free to install.

I suspect there was some trouble with your installation of KiCad V6. Maybe the libraries were not installed, or something else. If there is any problem with V7 you can always come to this forum for help. There are plenty of people here to give support.

1 Like

You can make a symbol for off-board parts and have a nice explicit schematic. Here is a battery symbol, which is excluded from the board (so no footprint) but not excluded from the bom so it can be ordered with the board parts (or moved to a higher-level assembly bom which includes the assembled pcb, enclosure, and misc bits). The board has a matching connector which can be installed or not.

Or use purely-decorative symbols that are excluded from both board and bom, just to make schematics nicer, like this switched-battery symbol or arrows on schematic block diagram page 1, or a pinout sketch for a modular connector:

1 Like

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