Top Ground Copper pour in PCB having three RF Sections

Question

I am designing my second RF board (First one had BLE). This board has LoRa Components (SX1257 and SX1301), GPS (MAX-6) and 4G LTE Module (SIM7600). All the components are on top layer (red layer).

My STACKUP is: Layer 1 (Red): Signal layer with Ground copper pour Layer 2: Ground Layer Layer 3: Power and Ground Layer (There are multiple sections for 3V3, 1V8, 4V and the section just below RF traces is Ground) Layer 4 (Blue): Mostly Ground having few signals.

Below is the picture of Layout:

My question is I can pour ground copper on my first layer with via fencing and stitching at a distance of wavelength/20. Should I keep the ground pour separate for LoRa, GPS and LTE module? They will be connected to each other via layer 2. Or I can have a big copper pour covering the top layer as distance with three RF section is sufficient.

Answer 1

My question is I can pour ground copper on my first layer with via fencing and stitching at a distance of wavelength/20. Should I keep the ground pour separate for LoRa, GPS and LTE module?

There are a few problems with separating ground planes:

Return currents on the ground plane have to travel back to the source via a different pathway (usually). If the rue is a high frequency current, if a trace crosses a slot in the ground plane this can add inductance to the transmission line or trace (so don't cross over the boundary of a ground plane with a high frequency trace or you'll suffer the consequences)

The separated ground planes make great dipole antennas. This is usually not a super big deal, but it can be if your trying to pass FCC testing, and you have a radiator that you didn't account for.

Seperated ground planes can also add inductance if the portion connecting them is small or through a via and trace on another layer (a bad idea in almost all cases).

If you need isolation or if parts require a separated ground plane (I've seen one GPS module that recommended a small one), then go for it and separate the planes. Otherwise a continuous ground plane is a good idea.

There has been a few times where I have used a slot to re route large return currents away from sensitive analog electronics, but that may be the only time I've found separating a ground to be beneficial (other than isolation)

Answer 2

The currents will be constrained to the area under the transmission line. You can just pour one copper. In addition they are in separate bands so even if they do interfere it will not necessarily give issues (After all, the antennas themselves will interfere anyways). The most important thing is to have good uncut grounds under the transmission line.

I have to say your lines connecting to those connectors look very thin. Have you checked the impedance?