Routing VCC with jumpers?

Question

I'm trying to route a new VHF RF receiver (LO is 151MHz, RF is 162MHz). There's a pair of LC filters on this board, as well as a Si5351 oscillator and a crystal. From what I've read, an uninterrupted ground plane becomes especially important when designing boards like these, and I'd like to make sure that's what I build here.

The problem is, my 3v3 VCC is on the left side of the board and it's needed by the Si5135 on the far right. I'm not able to move components around to bring these two closer together (I'm constrained by the microcontroller board I'm using and by the placement of the LC filters.)

Is routing power using jumpers -- say, 22AWG -- a viable solution here? A simple piece of wire would save me from routing the VCC line all the way across the board, cutting the ground plane in half, and it'd save me the cost of a four layer board. What are the up and down sides of using them?

Edited to add this layout: (with corrected uFL connector and unblocked references)

• Bottom right: RF section with LC band pass filter and uFL connector
• Top right: LO section with low pass filter, Si5351 and crystal (far right)
• Just left of center: NXP SA636
• Far left: IF section with two MuRata filters
• Top left: Demodulator section

Ground planes aren't shown, but will be on both sides of the board. Red traces are front side, green are back. The pinout is for Adafruit's "Feather" boards: Feather

---

Update, Feb. 6th: I rerouted the board along the lines of AnalogKid's suggestions and added vias as a'la TimWescott. (I had meant to add these but figured it'd just be confusing in the original post.) Here's the updated board:

I made sure that U1's decoupling capacitor is between the power supply and U1's pin 5 (the power supply line.) Is the trace there a little long? Either way, I think this layout is significantly improved.

I also added guard vias between the LO, RF, IF and demodulator sections. The pitch should be well under what's required for ~151/162MHz. I also added vias to stitch the front and back ground planes near just about anything marked 'ground', and added some on the "far" side of the 3v3 line on the rear.

Always looking for more info, but even if there isn't this was a huge help. Thanks!

Answer 1

Nothing will work as well as a 4-layer board, but if the costs are that critical then it is worth a try. The wire inductance will be larger than a trace on a pcb layer running above a ground plane. Be sure to have plenty of medium and high frequency decoupling as close as possible to the device pins. Also, the loop inductance will be larger, and the wire will radiate more.

I've seen this done with miniature coax, but my guess is that the added wire prep and assembly labor would cost more than the 2-layer / 4-layer incremental cost these days.

UPDATE: Now that you've posted the board, AND IF it is the green traces you want to replace, you can push most of them to the top side. many of your reference designators are blocked, so this will get messy.

1. Starting at the far right, bring the 3.3V via left to just above C11, and route a red trace to C2x pin 1 where the via was. Place vias above and below C11, green trace below C11, and red trace to the connector pin 2.

2. Red trace from the via above C11 to the left of C13 pin 2. Via and green trace below the trace from U1 pin 4, to the existing via near C17 pin 1. You now have two very small islands in the bottom side ground plane.

UPDATE #2. Instead of #2 above, run a red trace from pin 1 of the large round thing (electrolytic cap?) right of the connector, to U1 pin 5. Now the ground plane under the trace from pin 4 will be continuous, and there is only one short "jumper" on the bottom layer.

Answer 2

Something that I do on small boards, but haven't done with an RF board yet, is to stitch the top & bottom ground planes together with lots of vias, and if there's any part of a plane that's sticking out into nowhere, I try to put a via on the end of it.

BUT -- I haven't tried this with RF boards. I think that if you make sure that there's a good ground return path for every signal you should be fine, even if your ground planes are otherwise a bit cut up (especially if you use my stitching idea).

The thing that you really want to avoid is a ground plane with a critical signal running over it that just stops -- when that happens the signal current can no longer be mirrored by the ground plane, and you get an impedance bump.

Answer 3

To hold down the spurs at 120 Hertz on your Local Oscillator, you need to keep the reference (XTAL) oscillator edges clean; this requires you to keep magnetic fields away from the XTAL osc and from the path between XTAL osc and the LO synth IC; any logic gates or limiters or over-driven amplifiers act as mixers and will modulate any superimposed 120Hz onto the XTAL osc output as undesired sidebands. 120Hz fields can be attenuated by slabs of steel, or by distance; standard 35 micron copper foils will not attenuate 120Hz.

A key fact to use in designing low-phase-noise or at least predictable-phase-noise systems is this

Beta (the phase deviation in radians) = Delta Freq / Frequency of Modulation

For low frequencies (the Frequency of Modulation), the small denominator and a equally small numerator value will produce ONE radian of deviation. You don't want that.

To hold down the closein and the farout phase noise, you need to establish a "local battery"; this means have a voltage-divider (all filters are voltage dividers) with a series element of high impedance and a shunt element of low impedance. In this case, the series element is your WIRE. More impedance is better, because you'll have better filtering.

However that wire is also a target to pick up trash from any nearby circuitry. Just as a trace is a target. At least you can experiment with the LO purity, by moving the wire into other paths.

I'd use a RC LowPass, right by the LO IC, with 10 ohms and 10uF or 100uF. This 1 milliSec tau produces 160Hz corner, not improving the 60/120Hz rejection (an LDO is needed for that, after the RC LPF), but greatly reducing any switch-reg or MCU clock trash induced onto the "wire". To ensure the rolloff at high-freqs, consider this

^{simulate this circuit – Schematic created using CircuitLab}

Answer 4

Have you looked at routing the 3volt away from the rf