Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It only takes a minute to sign up.
Sign up to join this community
For example, let's say I have a power jack which is mounted on a panel and connected to the PCB using wires. I might also have a few 1/4" audio jacks also mounted on the panel and connected to the PCB using wires.
On the PCB they have place for the wires and not a footprint. How can I have these parts in the schematic and show up in the BOM and if possible the net list as well?
Create symbols for the off-board parts and define the type as "mechanical" parts.
You can choose "Standard", "Mechanical", "Graphical", "Net Tie (in BOM)", "Net Tie" or "Standard (No BOM)".
Show them on the schematic- using text etc. so they stand out if you need to verify or change them. They will then show up in the BOM automatically.
You can do a similar thing with mounting holes, except they would be "Standard (no BOM)".
You can also create parts and footprints that have no pins, which means that if you put them on the schematic they will automatically be transferred to the 3D PCB layout. This is useful for parts that you want to appear in the 3D model (and BOM) but have no electrical connections on the PCB.
If you are just using wires soldered into holes on the board, rather than connectors, to connect these items to the board, I would use any suitable footprint for the holes on the board - the footprint needn't bear any relation to the actual part, other than having the right number of pads. Associate this footprint with the schematic symbol for the off-board part.
You should probably have a note on the schematic that these parts are mounted off-board.
I use the same method Spehro described, except I create a schematic "component" with the type "Mechanical" selected, but I also add a graphic so that the person viewing the schematic can see what the external "mechanical" component is. I use this for fuses, socketed modules, hardware, etc. Example:
Schematic:
Component properties:
Note the "Component Type" is set to "Mechanical"
There is no footprint associated with this part, instead it is socketed in two headers. The headers have footprints but the module does not. Both the sockets and the module still show up on the BOM though.
In your case you can either create a footprint specifically for your power jack that is simply made up of the pads you solder the wires to, or you can set the component type to mechanical and place pads on the PCB manually.
