Single-Board Universal Module

I'm really excited about this project, and your efforts, and I like to add my two cents if I can make some improvement.

I'm not saying the design is not going to work, but "best practices" should be employed to minimize later head-scratching.

Most commonly done is pouring ground all over the top layer, via sharing is not a problem if you add sufficient amounts of them. Add a couple of extra ground vias on critical points, the current will follow the least impedance. More and larger is merrier.

4-layer RF wise is usually only different in that the RF circuit has a much thinner dielectric, making life easier with shorter/better ground vias, reasonable line widths, and of course more space for control- and power routing. 10-mil PCB's are not easy to deal with, and have to be supported.

I'm not yet convinced that a fat power plane is necessary when the current draw is weak, given a choice I'd make some room around the perimeter on a power plane for signal lines rather than have these cut off continuous ground paths. (the Cypress reference has a power bus.)

On this board there is not much sharing between the four chips as only one is used at a time, so sharing would be limited to between the RF-generator, switch, PA, and low pass filter.

The manufacturers recommended layouts should be safe bets, I asked the NRF people about their layout and it turns out that grounding of their chip is non-critical as its output is differential. The same holds for the other parts. Cypress offer a very nice guide and layout examples. www.cypress.com/?rID=34190
Ground vias under the RF chips also have the function of conducting away heat. They will also wick away excess solder paste to keep the part from floating away from connections, and will pull the part down to the board. Sounds simple but I've been surprised some very talented people have missed this.

No doubt many RF PCB designs have a lot of overkill, which is the fastest and most economical way to solve the design issues. If you have a resource for free then use it.

I'll take look at submitting a board design, but as a variation on yours, as I'm clueless (almost) on the digital parts.

Sorry stating a lot of obvious things.

What TI are saying is to not short power pins together and then add the caps like a gang, each pin should have its own cap and ground via(s). This is to create some isolation between different parts of the die.
Noise would be a bigger problem when the chip is used in receive mode.

The TI 2500 design has thermal reliefs on all components, while this may very well work, it does not improve RF performance, but is of course to make reflow process easier, with less tomb-stoning etc. For a small board like this I do not think tomb-stoning will be a problem at all.

Their layout should be adaptable in this design. It does not look too sprawled out.

TI layout AN098

p.7

11 Verify that the top ground pours are stitched to the ground plane layer and bottom layer with many vias around the RF signal path. Compare to the reference design. Vias on the rest of the board should be no more than λ/10 apart.

λ/10 at 2.4 GHz should be like 12.2 mm. Considering the velocity factor for a PCB with DK of 3.67, (1/sqrtDK) ~ 0.521 this 12.2mm shrinks via spacing to less than 6.4 mm apart.

I don't know what the shield physically looks like, but perhaps its footprint should be made into a part, to make it easier to move without mangling it.

That shield eats a lot of space, it would be good to find out if it is really needed.
If so Laird has 32x32mm and 26.21x26.21mm shields with snap on lids, but I can't locate this rectangular shield. The Laird shields are good and not too expensive

I'm not sure of all the mechanical constraints, board dimensions, JP2, and the four mounting holes? Can U.FL be moved to the other side, a corner notch could added for the coax routing?
Do you have .step file of the housing this board fits inside, or some approximation?
The four mounting holes (which I think should be vias) and JP2 could be made into a library "part" to keep them together, avoiding the risk of them getting pushed away. It looks like this board vendor can do vias at this size, which will be a perfect grounding for the PA and antenna.
I normally do not add a "route" to the ground side of decoupling caps etc, the polygon pour takes care of that. Moving a ground via with strings attached can lead to mistakes. I'm using the demo version so I will not be able to submit a 4L design.
I'm getting a few DRC errors.

Getting a custom shield made will cost a few grand to tool up. If the 32mm shield can be used, perhaps just punching a hole in the lid for JP2, if it would ever be necessary, could work. The main reason I can see would be the keep RF from feeding back from the antenna to the input. At +2dBm like many of these modules put out this may not be a problem, but at +20 it may be different.

R/C Transmitter units often have the TX module under a shield. I doubt they want to waste money. Some FCC and ETSI regs may impose some emission- or susceptibility rules that forces this.

I looked at the last version, added some changes.

32 mm square shield would necessitate a U.FL thru hole, I see that.
IPX is "100% compatible" with Hirose U.FL and has a thru hole version.
rfconnector.com/ipx-connectors.php

Perhaps not a big deal?

The weak signals with vias in oscillator crystals worry me more. These has not given you any problems? For ~$1.5 you can get sub 25 ppm powered XO's. The 12MHz can be shared.

It helps to have the whole picture, I can see two of the mounting holes fit outside the shield, but I wonder if the top can snap off, if the screws can't be installed under the shield?

Higher density connectors can perhaps be considered (0.050" pitch)?

The PPM connector is only using 3 pins, maybe a four pin connector could be used to free up space (of pin 5)?

The 10-pin connector has four unused pins, could these be used the micros pin 37, and 44, 2 x 2 pin connectors?

Well, I'd thought I'd ask anyway. I don't have all the details.

Nice job cramming all the parts into the smaller shield!

The output line should be re-routed under the gap in the shield.

The polygons under the switch probably do not help. Its all ground anyway.