I want to use a MOSFET that has 8 pins. Pin 5-6-7-8 are drain, pin 1-2-3 are source and pin 4 is gate. I’ve downloaded the symbol and footprint. Footprint is nice but the symbol has 8. I want the symbol to be a regular NMOS symbol with three pins only in the schematic editor but Kicad must know some pins are connected otherwise it doesn’t let me connect internally connected pins in PCB editor. How can do that?
I named the pins as on the left but in the PCB editor on the right, I am faced with “unconnected”:
In the pin properties window click the ‘visible’ box. Generally the pin to be hidden is placed on top of the visible pin to keep things neat. Once hidden you would not know it was there except in the editor.
Putting the pins on top of each other worked, I didn’t need to make other pins visible. The thermal pad was defined as a solid on front copper layer but not a pad that’s why Kicad refused to pour copper. I copied pin 5 and scaled it to the exact dimensions of the thermal pad then deleted the original thermal pad. It looks like a crude way but it works, even the DRC errors are gone.
For ICs with thermal pad I add a pin with number 0 and connect it at schematic to GND.
If the case have thermal pad by default connected with pads 5,6,7,8 then it really is one complicated shape pad and not separate 5 pads. I would consider making a new footprint having only 3 pads.
Pads 1,2,3 will get for example all number 1, pad 4 will get number 2, pads 5,6,7,8,0 would get number 3. If typical MOS symbol has different numbering (need to be checked) than may be 1,2,3 in different order.
Putting pins on top of each other is called “pin stacking” in KiCad, and it is a valid and common way to do things, even though I do not like the method much personally.
Another method is to change the footprint. As you have already discovered with pad 5, in KiCad, pads with the same pin number have to be connected on the PCB. So you could also use just 3 pin numbers, and use the same number for multiple pads. You can even take this a bit further. KiCad do not have to be numbers, but can also have letters (or a combination). You can use the pin “numbers” “G”, “S”, and “D” in the schematic, and use those (and only those) numbers in the footprint too. This method is used extensively in KiCad’s default libraries. Just look up any footprint with the keyword “thermal” in it.
