PCB RF Layout Critique: Input on my radio-telescope PCB

Question

I'm attempting to do the board layout for a radio-telescope we're building at one of my jobs.

Here is the overall system topology:

^{QRFH is for "Quad Ridged Feed Horn". It's a rather esoteric antenna type.}

Basically, the intention is to allow extremely high-precision measurements, with in-situ calibration and drift tracking. There is a built-in system for measuring antenna SWR to calibrate out drift due to physical changes from temperature changes, calibration for the SWR calibrator via the ability to feed the SWR oscillator directly in to the analyzer, a optional pilot tone to allow for tracking oscillator drift in the spectrum analyzer, a noise diode, termination, and a small dipole for measuring local RFI.

Complete PDF of everything here

Anyways, here is my current layout:

Updated Layout:

Original layout:

Stackup:

Top layer:

Ground 1:

Power and interconnects:

Ground 2:

Overall view:

All transmission lines should be within ~1Ω of 50Ω, taking the dielectric of the FR4 from the board house I intend to use into consideration.

Right now, this is intended to operate in the 50-300 Mhz band, so more esoteric dielectrics aren't really warranted, but I have them under consideration.

LNA Amplifiers are mini-circuits CMA-5042 with TCBT-14 bias-tees.
ESD protectors on I/O is via CLM-83-2W+.
RF Switches are JSW6-33DR+ (the 6P switch has better performance then the 2P switches, so I'm using a 6P switch in the 2P switch position as well. The price difference is negligable).
Variable attenuators are all DAT-31R5-SP.

Basically, I'm seeking a few things.

• Does my layout at least look mostly sane?
• I have switch and attenuator control traces running under RF traces, albeit with a ground plane in-between. I don't think this is an issue, but RF is weird.

I've kept the soldermask back from all RF transmission lines as much as possible, with just little barriers around the SMT parts to prevent the solder from running down the traces.

Mostly, I have just not done RF layout before, so I appreciate any input.

Answer 1

Here are my thoughts and concerns, based on lots of practice and mistakes in designing 902-928MHz ISM band products on FR4:

1. Definitely consider through-hole RF connectors, as The Photon suggests. SMT connectors break off easily taking part or all of the pads with them and often strip off a fair amount of the center trace. The embedded vias provide little additional strength: you're talking about a few thousandths of plated-up copper gripping the very edge of the pad that is only a few thousandths thick. Time spent milling out clearances will pay off the first time that cable is yanked hard... only the cable will require replacement. I refuse to use SMT connectors for anything, hard experience makes me do this. An alternative to vertical or pagoda style connectors are the edge-mount variety. These have no mounting holes and are "surface mount" but solder to both the top and bottom side. I've never broken one of these or pulled one from a board.
2. Hot-plate soldering both the small RF components and the large connectors is likely to overheat the smallest components while waiting for the big brass connectors to heat up enough to reliably re-flow, especially the center pin that is buried inside of all that brass and PCB. Consider hot-plate soldering only the small SMT and then hand-solder anything big. Thermal reliefs in your pads are always a good idea for even and reliable solder flow. I use them on RF connectors for 902-928MHz boards with no ill-effects; their presence is not measurable. The thin gap only needs to be the minimum required by your PCB vendor and you can use multiple thermal legs. Vias in the connector ground pads will make the connectors much harder to solder. Consider moving them just outside of the ground pads with one at the end of each copper bridge across the thermal gap.
3. Your estimate of 1% impedance is very optimistic. 5% is possible with FR4 if you can spend a few board revisions tweaking trace widths, materials and the fabrication process until you get the right recipe. Otherwise 10% is more the de-facto standard for a vendor's standard-process PCB fabrication. Keep in mind: a. That the press pressure used to laminate the board can have significant effect on the finished layer thickness, especially if the layer is made of pre-preg. Try to use core material for the controlled-impedance layers because it is not affected as much by pressure variance. b. The location of your PCB in the large fabrication panel (at center vs. at panel edge) will change the laminating pressure, as will its position in the stacking of various PCBs all being laminated at the same time. Working with a PCB vendor we ran RF test coupons at the center and corners and found significant differences. c. Trace width tolerance is given by your PCB vendor based on their experience with their etching and plating process. Calculate the effect of min/max trace width on your characteristic impedance. Wider traces have less sensitivity to the fixed trace width variance. d. The dielectric constant of FR-4 from a single manufacturer can vary considerably from lot to lot and depending on the glass/resin ratio of the prepreg or core used in each layer.
4. The characterization trace is only accurate on the vertical segments yet your actual circuit traces are primarily horizontal. The warp/weft of the FR4 can cause measurable differences in impedance depending on trace direction, though less so as frequency decreases. You don't say if you are using a TDR or VNA to measure the impedance, but either one should do fine with a simple trace straight across the board. If you want a longer trace, serpentine the straight portions in the horizontal direction instead of vertical. Try moving T2-A up and T2-B down to make this work better, if needed.
5. Watch for coupling between parallel RF traces. I don't know if the various sources are always on. When a source is not selected, it is reflected back from the SP6T RF switch which leads to standing waves and maybe unexpected results.
6. Make provision for a metal shield to enclose the circuit.

Answer 2

At a previous employer, it was considered good practice to throw 2 or 3 stages of RC filtering into the control lines of any switch to prevent any noise coupling into the output signal through the switch control lines. 700Hz corner freq or therabouts.

^{simulate this circuit – Schematic created using CircuitLab}

From a Schematic point of view, you look a little light on bypass capacitors and filtering. How clean are the 3.3V supply rails?

From a layout point of view, it looks pretty good. Keep in mind that transmission lines aren't really effective for short runs compared to wavelength, so you're probably fine there.

Answer 3

You might want to add a thermal release to the connectors.