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?
1 Like
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.
1 Like
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.
1 Like
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.
Doh!
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.
1 Like
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?
Is this the proper way? hidding the pin (it’s pin 49 near pin 13), and how i make this pin connects automatically to GND on the footprint?
Also im following the Library Convention, but i can’t set the grid to 100mil, so i make it on 50mil.
I want to make this best i can, i want to share it to the other users.
Thanks in advance.
Carlos
I’ve seen other symbols define the EP as a Passive pin an not a Power Input.
