Hi all,
i m quite new on this and I have been trying to solve an issue which might not be an issue at all, so please throw some suggestions.
Some of my schematic components will be off-board (switches, potentiometers, etc). Thus, I have assigned connectors as their footprint (eg pin headers). So far so good.
When KiCad populates the PCB with the footprints and nets, it follows a 1-to-1 relationship, so that pin 1 of the off-board component, will be connected to pin 1 of the pin header layout and so on. However, when I start routing the board, I realize that routing would be much easier and cleaner if I could reassign the connection between the off-board component and the pin header. Let’s say pin 1 of the off-board component should be assigned to pin 5 of the pin header layout.
As I understand one way to solve this is to move all off-board components to a second hierarchical schematic sheet and do the rerouting there. This feels ok for things like buttons, connectors etc but it doesn’t feel ok for eg 3PDT switches since switches are vital components for a schematic as they affect the functionality and they are not just an interface.
The second way I see being proposed a lot, is to edit the pin header footprint and rearrange the pin numbers which solves the problem but the result seems irrational. My brain denies the fact that I will need custom header footprint everytime there is a pin which is easier to route if it sits somewhere else. It also looks pretty bad since the pin numbers are out of order.
So, is there a way to manually assign schematic component pins to layout component pins which is neat? Am I missing something here?
So, is there a way to manually assign schematic component pins to layout component pins?
No. The connection between symbol pins and footprint pads is done according to the pinname<–>padname (number) assignment. This is fixed, there is no connection matrix inbetween to change this assignment.
You have to redraw the connection in the schematic according to the wanted connection.
small note: it’s best to use the exact kicad description strings if you want to describe something. I have interpreted you question this way:
schematic component pins → symbol pins
layout component pins → footprint pads
Hi @mf_ibfeew thank you for the clarification of the terminology, I was also wondering if the fact that I cannot find what I want is because I lack in the terminology.
As for the solution, unless I am missing something, redrawing the schematic is not possible when talking about switches as redrawing the connection will lead to a different functionality. What i can possibly “redraw” is the numbering of the symbol pins. Is that what you mean? Is this considered a “neater” solution than changing the numbering of the footprint pads?
The third way.
Accept the fact that KiCad is the PCB design tool and not the device design tool.
Your components being off-board are part of device but not part of PCB.
If I place connector at PCB then I have connector at PCB schematic and connect wires to its pins as I need.
That way I also get this connector in PCB BOM when I order PCB to be assembled.
Changing the pin numbering in the schematic symbol is more common then changing the footprint numbering. In the schematic they are “just numbers”, while in the footprint, the pin numbers have a logical order / meaning.
I’m not sure why you would choose to change a footprint’s pinout in this case. It is far easier to just re-order the labels or connections on the connector schematic symbol.
When I want to re-map pins, I put Schematic and PCB side-by-side. Then, I remap the labels in the schematic and F8 to push the changes to the PCB. It is quick and simple.
I am not following this logic. Re-mapping the pins in the schematic is the same whether the symbols are in a hierarchical sheet or not. Again, this seems like unnecessary steps.
You have a connector (socket) on the PCB. You have the other part of the connector (plug) that is attached to the off board components. The two parts match each other (male pin 1 to female pin 1 etc.).
As @mf_ibfeew says, you redraw the Schematic. The parts you redraw are the wires between the off board components (Pots, switches etc.) and the off board half of the connector. You do not redraw the Schematic that becomes the PCB.
Eg. Let’s say you attached the three pins of a pot to pins 4, 5 & 6 of the connector, but track laying would be easier if the pot was connected to pins 1, 3 & 9. All you do is redraw the wires from the pot to the different pins on the connector.
This is a really common procedure that is frequently done to help ease PCB routing.
