I’m using some of these very common four-pin NO tactile switches where pins 4 and 3 and pins 2 and 1 are internally connected like this:
Which symbol should I use? If I pick a SPST I’ll end with two pins only but I’ll need four of them on the footprint for the PCB. If I pick a DPST switch I’ll have to manually connect each couple of pin.
What’s the best way to deal with such parts?
In my opinion both options are OK. When I choose SPST I also renumber the footprint pads in order to have two pads number 1 and two pads number 2.
Unfortunately kicad is not aware of the internal connection.
The footprints for such parts in the official lib are setup to fit the spst symbol (they have the pads doubled)
You can of course make your own symbol with your own footprint that has all 4 pins with separate numbers. This will give you a bit more control over what needs to be connected. The symbol could look like this:
I advise against using the dpst symbol as it represents something very different.
This is my opinion; I dislike @Rene_Poschl 's approach because switches come in a vast variety of physical form factors. There is no need to convey this information in the schematic.
What you have is a NO SPST switch. There is no need to do anything extra on the schematic just because of the information on this particular datasheet.
And here is the Footprint:
OP if you had done the naive thing and picked a NO SPST symbol, then when it comes to choosing the footprint you will see there are suitable ones for this kind of switch with duplicated pads, differing only in the button height which affects only the 3D rendering. It just worked for me. Praise be. 
In a little different occasion I have mentioned that problem (discussed here regularly):
That approach servers different use case. As Rene said: “This will give you a bit more control over what needs to be connected.”
I had to use that approach because I had severe space limits. I had no better option than to rely on the internal connection of the switch and leave one pad unconnected. I used a 4-pin symbol for that. Otherwise I would have needed to connect all pins on the board and I couldn’t have done the other routing.
I, too, (along with Piotr) would like to see this problem solved in some way in KiCad. Needing 4-pin symbol for 2-pin functionality feels clumsy.
Electronics frequently deals with one signal connected to several pins or components with internal
ly connected pins. BGA have dozens of GND what is the very same situation and nobody complains about. Stumbling above the LT1790 voltage regulator in Kicad symbol library shows another dirty attempt to workaround the missing multiple PinNumber feature of Kicad. The LT1790 has two GND pins (pin 1+2) connected to the substrate to meet datasheet specifications. The symbol is 3 pin what allows only one GND wire in schematic. To generate correct netlist, second GND pin is placed unvisible over same pin symbol coordinates than visible one. Maybe we should think about written library conventions about to treat this for the diffrent requirements.
These are our current rules. We can stretch them a bit but to be honest most of it is non-negotiable at this point in time.
I wouldn’t say it’s the same situation. For example a physical switch could be changed between board versions (any two pin or internally connected 4-pin would do) but the symbol could be kept the same. And you wouldn’t expect to be able to route only one GND pin of such a BGA package, would you?
@Rene_Poschl Remind me please; does pin-stacking on the symbol work to solve the issue of two(2) GND pins on the LT1790 mentioned above?
Stacked pins guarantee that their respective footprint pads are connected. They allow the use of generic footprints while still allowing to have such a connection made.
This is why we typically require pin stacking for ground pins. We allow the positive supply pins to stay separate as it allows the user to indicate which decoupling capacitor goes with which pin.
There are also applications where stacking is the best option when considering ERC. An example is a power supply with multiple output pins of the same potential. When the pins are not stacked then one would either need to give all of them the type power out (resulting in false positive ERC reports) or have some of them with a different type (resulting in ERC possibly missing a true error)
Thanks for helping! I’ll go with a SPST switch and choose a suitable footprint.
This is different situation. I have not used BGA, but when I have a microcontroller with several VCC/GND pin pairs I would never used only one pair to supply it mainly because of disturbance generated by current pulses taken from supply having in mind the internal connections betwean pins and structure. If I/O pins would have to use supply pins from opposite case size the current path would be longer and return path would be less parallel (in current fast switching ICs it is important). All that has nothing to tactile switch. Connection in tactile switch is strong enough to not need an additional track out of it. The same is for:
https://www.digikey.com/product-detail/en/panasonic-bsg/BR-1632A-GAN/P291-ND/447502
addition connection by traces will not make the connection better 
I’m not sure if it was said here that if KiCad would need you to connect at PCB already connected tactile switch pins and it would disturb you you can add more layers to PCB and made that connection at one of them and then just not generate gerber for that layer.
Is a dirty hack that works for tht. To be honest if that is a concern than i would go with the symbol i present up top and have it properly documented in the schematic what should be left unconnected. (will help you remember what you did sometime down the road and also works for smd)
I have written that because OP showed THT switches and decided to use SPST symbol (I understand it is the symbol with 2 pins only).
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
