I have a boost converter that requires 2 GNDs, separate on the top layer but tied to the same GND plane on an inner layer. On one of them I’m using the GND net, same as on the inner layer so it isn’t an issue. The other I’m using AGND as the netlist name so that when I do a copper pour on the top layer to cover the whole board this will remain as an island, only connected to GND plane with vias. But then I can’t actually get the via to connect to the GND inner plane as they’re different nets. I don’t think net ties are what I want as I don’t want to connect them on the top or bottom layers, I want to connect them through a via as if AGND was GND for everything other than when I do the top layer pour.
Good GND layout for an SMPS is important. What you are attempting to do is very likely a very bad idea.
But if you persist…
I think you can use a THT pad as a net-tie, and then assign multiple nets to that THT pad. I think this was new in (maybe) KiCad V7, but I have not used net ties for a while and am not sure about the details.
Could you please elaborate as yo why it’s a bad idea?
I’m following MAX77801’s datasheet wherein the layout example says
“AGND must carefully connect to PGND on the PCB’s
low-impedance ground plane. Connect AGND to the
low-impedance ground plane on the PCB (the same
net as PGND) away from any critical loops”
So I was going to keep AGND as an island not incorporated into PGND’s pour which will cover the top layer of the PCB and connect the 2 with vias onto a common GND layer
I just don’t see how this fits in with the board stack-up I was trying to make with a solid gnd layer, they’ve just routed between the two rather than using a plane.
Should I create an agnd island on the gnd plane too and then use a net tie to connect that to the rest of the gnd layer? Also is it possible to place net ties on internal layers?
With everything being said here: Most of the time the easiest solution is to have one GND pour for everything which also produces good results. The important part is to keep the traces on the switching node short and wide, make sure the feedback does not directly cross this switching node and that noise-suppressing components are placed close to the noise source. Having a split GND which is then connected with vias won’t change much.
Looking at the image posted here I can understand the design if you have a two layer board. As soon as you have more layers, I’d use one of these layers for a full GND pour, while also having the two (AGND and PGND) pours shown in this image. The connect both of them to the internal GND layer with plenty of vias.
After looking at this graphic a bit more, I think this is also exactly what is done here, see all those vias? I’d bet that the net tie shown here is only to understand that it has to be connected, while also having a solid layer
You have two options: either do what you think is best or follow the manufacturer’s recommendations. Perhaps a third option would be to do a mix of the first two.
If you’re not sure (conservative mode), I would follow the manufacturer’s recommendations, as they surely know much more about their product than most people on this forum. This way, you can also ask for support with more confidence if, unfortunately, something goes wrong with your design.
Getting back to the matter at hand… If you want to replicate the suggested layout, simply grab a net-tie from the kicad symbol library, place it in the schematic connecting AGND and PGND, assign a net-tie footprint and continue with the layout routing. You will have AGND and PGND nets in order to create respective zones/islands.
