Some components, like for example most SMD crystals, have ground pads which have no representation in their schematic symbol.
Right now I associate a 3 or 4 pad footprint with the 2 pin schematic symbol and then assign GND net manually to the respective pads during layout. However, when after changes to the schematic I recreate and re-import the netlist, the manual assignment of GND is lost. This is easy to miss when one is in a hurry to respin a board, especially when relying on ground fill to connect the pad.
Is there a way to “hard-wire” pads in a footprint to GND? Or is there a “proper” way to handle these kind of pins?
I’m not sure about a “proper” way to do it, but I would always default to re-doing the schematic symbol to show the additional pad. The pins on the symbol don’t really hurt anyone and it will guarantee that an error/warning is thrown when you associate the footprint and don’t connect it in the layout (especially if that extra pad is assigned to ground).
As for the “hard-wire”, I’m not sure if it’s possible (maybe if you edit the footprint file?) but I think that would be dangerous either way. I imagine a situation where I hardwire a pin to “GND” and then in a layout down the line, I have both “GND” and “DGND” nearby one another and I mistakenly hook up that pad to GND when it really should be on DGND. Niche application perhaps, but I’d rather be explicit with the footprint/symbol combo.
Good point about multiple grounds. Being an amateur as far as EE is concerned, I was looking around for example schematics and am surprised how uncommon it is to show grounding for the crystal resonator.
One thing that was surprising to me when I was starting out (and continues to surprise me) is that in any CAD program (KiCad included), there is never a “one size fits all” solution for footprints and symbols. Sometimes you are forced into this by a company, when everyone is expected to be using the same stuff; even then, there will be variations.
My suggestions are to learn the process of making footprints/symbols, cultivate your own libraries (because that’s the only way to be sure something is right/verified) and keep a simple set of rules about how you will organize the library and create the items within it. It stinks at first, but a good library is an asset that allows you to make designs quicker in the future.
To answer my own question: Power pins (incl. ground) invisible in the schematic can be defined with the symbol. In the component editor, add a pin, give it the name of the desired power port (e.g. GND) and clear the “visible” check-box. Don’t forget to set a pin number matching the footprint.
These pins won’t be visible when using the symbol in a schematic. In Pcbnew the respective pad will be connected with the power port’s net (as long as the power port was included into the schematic).
In my case, I copied the crystal component and created CRYSTAL3 and CRYSTAL4 for 3-pin and 4-pin crystals with 1 and 2 invisible GND pins respectively.
Greetings, sorry for ask on this old question but i didn’t want to create a new post if all the information is here. I’m starting to use KiCad, i’m making a symbol for the nRF51422 uC of Nordic Semi, and had the same question of Chicken, how to represent the exposed pad on my schematic?
