No not at all.
Around these pads there should be four, (one at each corner) thin connections to the ground plane. This provides thermal relief, so the ground plane is not going to suck the heat away from the soldering iron, or solder wave.
This is something I just can't figure out. The image from Hardware Design document (p.50) shows the exact opposite.
Does it make sense to widen UART traces?
To reduce inductance, resistance, etc.
I had to route RX and TX relatively "long", about 10cm.
My standard width for non-power traces is 0.25mm
But the words on page 49 say:-
- Put enough GND vias around RF traces.
In RF terms this is a long way. I would at least put a guard track around these traces.
I figured these must be two different things.
- I've separated the RF trace quite well, there is GND pours on the bottom and on the top side also, they are connected through vias.
- As the picture in #22 suggests, I used solid pad connections for the two GND pads on the left and right of the
RF_ANTpint.
So no thermal relief, how are you going to manufacture this? Solder wave or hand soldered. Either way you are going to have problems.
What about the guard track I mentioned? Do you know what this means?
Solder wave.
I think I know what you mean, but the GND pour on the top side should do the job, right?
And I routed the UART RX-TX lines as far apart as possible.
Wrong.
A guard track runs along one side, or better both sides, of a track you want to protect and isolate and decouple from the noise on the ground plane.
I see.
Both sides of the track and both side of the PCB?
But the guard trace itself should be connected to what?
To the ground at one end only.
I see, like a shielding of a standard cable.
And also the bottom side ground plane should be cut off under the UART RX-TX traces?
Only a return path GND trace beneath the signal trace?
Yes.
Yes. I think you have got it now.
Honestly, I'm not entirely confident in what I'm doing. 
I've cleared the GND planes around the UART RX-TX and created the guard traces on the top side (all of which are highlighted in the picture).
But where am I supposed to connect the return path? Is it okay to connect one end to the edge of the ground plane near the SIM modem and the other and to the ground plane around the uC?
(only RX return path is created for now)
Not quite sure what you mean.
If it is the guard track for the RX, then connect it to the same point as the TX guard track, that is at the main logic board end.
The trace between chip and aerial connector is a transmission line.
It must be of an exact width, spacing and type of circuit board material.
Got it wrong and the reflected energy from the transmitter chip will burn out the power stage.
There are online tables to calculate exact width and spacing, or follow chip manufacturers recommendations.
RF traces is dark art for the inexperienced.
Leo..
I meant the current return path, because the ground plane is interrupted. But probably the return current of RX-TX wouldn't want to flow back under the RX-TX lines anyway, since these signals are not very high frequency and the return current will take the least resistance path (not the least impedance).
Do I need guard traces on the bottom side as well?
Yeah, if you look closer on the PCB there is a fifty-fifty sign is hidden. It either works or it doesn't.
As you said, this is new territory for me, I could only rely on the SIM7070 Hw design guide:
RF traces layout
- Keep the RF trace from module ant pin to antenna as short as possible
- RF trace should be 50 Ω either on the top layer or in the inner layer
- RF trace should be avoided right angle and sharp angle.
- Put enough GND vias around RF traces.
- RF trace should be far away from other high speed signal lines.
- There should be some distance from The GND to the inner conductor of the SMA connector. It is better to keep out all the layers from inner to the outer conductor.
50 Ω termination will be in the GSM antenna.
No, that is the whole point of a guard track.
This is very very true. It is not something I would attempt to do. Even with the test equipment I used to have access to, it would take many iterations to get it right.
The first thing you need to do is to specify the type of PCB material you are going to use. Because that will determine the impedances of things.
Which you didn't do. Milimeters count at cellphone frequencies.
A wrongly calculated RF trace that long could comprimise the range of the module.
The Pi filter in that trace is equally critical.
Leo..
Thanks for pointing this out, it could be improved with some rearrangement. I will do that.
Hw design document doesn't put too much emphasis on this. Just 0R and NC capacitors.
I already use SIM7080 breakout where this "complicated filter" is implemented.
