Hello,
In a project, it is common that some components must remain off PCB : potentiometers, switches, jacks, LEDs, etc … These components will take place on a front panel and connected to the PCB by wires(via connectors). How to tell Kicad that these components should not be implanted on the PCB ? It is however essential to represent them on the schematic for a better comprehension. Is there an action ?
Thank you in advance for your help.
KiCad is not really designed for creating system design drawings.
The only option i can think of is to use # as the start of the reference for parts that are off board. This will however mean that these are not included in the BOM.
A better solution might be to create separate drawings describing the system instead of having everything in one “file”. (In profesional environments software like eplan is used to create these system level drawings. Sadly i do not know of an equivalently powerful open source tool. So you might opt to use kicad for these schematics only drawings as well.)
Wouldn’t that be a use case for a ‘virtual component’, or is that feature now otherwise used?
[edit]
OK, forget about it.
Just recognized, that those bulkhead/off-board components have no physical appearance THEMSELVES on the board at all, but will already be represented by connectors or other things… So yeah, VCs do not apply.
KiCad has no virtual flag for symbols. It has such a flag for footprints but that only excludes it from the position file. (pads would still be created for it. Or if there are no pads then netlist import will complain that there are missing pads in the footprint.)
You’re too fast for me slow brain 
I don’t see a problem here. They can be thought of as normal components, just with longer, bendable pins. Attach a proper connector footprint to the symbol. KiCad is nice and lets you choose the kind of footprint you need, you don’t even have to make anything new.
Qelectrotech is a worthy, free, system level drawing program. I am not sure how it compares with eplan but it can manage system drawings and comes with a fairly comprehensive library.
https://qelectrotech.org/index.html
https://qelectrotech.org/gallery/
https://www.youtube.com/user/scorpio8101/videos
A true system drawing would not only include the part that is off board. But also the connector soldered to the board, the connector on the cable, the cable and its color or number assignment, …
As far as i understand the request by @botanicus i would guess they want to have at least the connectors and off board components visible.
Yes, I missed the “via connectors” part and thought of wires soldered to the board.
That is one good approach. I used this approach when making my first PCB in kicad in 2018, following 0yvind Nydal Dahl’s original 5-minute tutorial video at https://www.youtube.com/watch?reload=9&v=l9b_6WLemmg
However, this type of pin/header connector is very easy to pull apart. If you want a more secure connection for an off-the-board component, the other two methods you should consider are:
a pad or a via that you can solder a wire directly to
a terminal connector (the footprint is already in the kicad 5.x library)
for example a 3-wire terminal connector for a potentiometer
Soldering the wire is cheap because you don’t have to buy an extra part, but not cheap because it takes a lot of time and effort to connect and disconnect the component. However, you can also just cut the wire if you ever need to replace the component and reconnect a new component with a lineman’s splice in the wire.
So you should carefully consider how securely attached to the PCB you want the component to be, and if you can’t decide, go with the terminal connector. However, with a terminal connector, you also have to allow room inside any enclosure to fit a screwdriver. Otherwise, it won’t work at all.
And as Rene already said, with these three methods the off-board component will be missing from the BOM.
The main alternative I can consider is to utilize # as the beginning of the reference for parts that are off board. This will anyway imply that these are excluded in the BOM.
A superior arrangement may be to make separate illustrations depicting the framework as opposed to having everything in one “document”. (In professional situations programming like eplan is utilized to make these framework level illustrations. Tragically I don’t know about a proportionately amazing open source apparatus. So you may pick to utilize kicad for these schematics just illustrations also.)
I think one of possible solutions can be to have one schematic of PCB (giving you BOM for PCB) and second at which PCB would be an element (can be defined quickly as new symbol) giving you a BOM for device.
Hello,
Thank you all for all these suggestions!
I will think about the best solution.
The method of # in front of the references seems to me well.
Solutions with 2 schemes is good too; pity that we can not save 2 versions of the .sch file (as with other software: “File / Save As …”). And the only export option is “Draw in the clipboard”, which can be recovered as an image in a photo software …
Regards,
Botanicus
[Translated from french by Google]
An advanced trick that I used for a project that has since been shelved was I created a hierarchical schematic with each sub-sheet an intended module. This allowed me to show the relationship between the various parts. I then created another project file in the same folder for one of the subsheets and made a PCB from that. Here is the project folder if you want to see how I did this. The ProtonPackCircuit.pro project file is for the full project, and the PowerCell.pro project file is for just the PowerCell sheet. ProtonPackCircuit.zip (2.4 MB)
This was for a friend through my local maker group for his cosplay GhostBusters Proton Pack. I intended to eventually do two PCB designs, but the he realized that this solution was too expensive for him and I only got one of the boards designed. The other board would have been for the Cyclotron.sch sheet. While I was disappointed that he didn’t want to follow through with this design, I wasn’t too chuffed as it gave me an opportunity to develop this project technique with KiCad.
I can get the full project BOM from the top project, and board specific bom and layout files (using a plugin, see the bom folder) for each individual board design.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.