Electronics > RF, Microwave, Ham Radio

Help me improve this power splitter

(1/6) > >>

tszaboo:
So I made a passive power splitter. It's part of my monthly JLCPCB designs, that I do for fun/learning. Trying new things.
It's made on the JLCPCB 04161H-7628 stackup, 4 layers with 2 grounds (and some stuff on the bottom side)
Schematic is 3x 16.5 Ohm nominal (16Ohm actual) resistors in a Y connection.

Now the bad part:
I measured it with a Megiq 440 VNA. The nominal gain should be -6dB, I got -6.5dB
It's relatively flat (+/- 0.5dB) up until 2.7GHz, where at 3.2GHz it drops to -9dB.
I'm trying to figure out what's the reason for this low bandwidth limit.
I have some suspects, but I wanted to ask your expert opinion before making a bunch more prototypes.
Theories:
-trash quality Aliexpress SMA connectors
-the middle of the Y connection isn't 50Ohm, so the separation should be different for the coplanar wavegide to match it
-0603 resistors are too big, should be 0402
-Something something VNA isn't set up correctly. I calibrated it with a Female SMA kit with a calibration quality adapter. The cal kit is~400 EUR.
-SMA end launch transition is bad
-Since I only have a 2 port VNA, I terminated the other SMA with 50 Ohm, something is up with this. Maybe I need to have a cable here.
What do you think? Any other theory?

mankan:
I'm no expert in this but I have some experience and a few comments, questions and tips anyway.

6.5dB, check any commercial splitter and they state IL of 0.2-0-5dB depending on make and model, that means in addition to the theoretical 6dB. So I would not worry about this.

What is on the bottom side? It ought not to matter but I'm curious.

VNA measurement setup: you should be fine. A normal thru calibration is all you need for this, as long you do not want to measure phase imbalance between the ports.

Resistor size: yes, smaller would be better. Some say you should mount SMD resistors upside down to reduce parasitic inductance. I have not tried this myself.

Board size, I would try to make the board much smaller. There is always losses in the PCB.

And finally, I guess you have multiple boards? Mount two 0 Ohm resistors or small capacitors (100pF-1 or 10nF) and cut off the third trace close to the middle and measure the loss, this ought to give an idea of the PCB losses.

RFDx:

--- Quote from: tszaboo on January 10, 2024, 02:26:37 pm ---I measured it with a Megiq 440 VNA. The nominal gain should be -6dB, I got -6.5dB
It's relatively flat (+/- 0.5dB) up until 2.7GHz, where at 3.2GHz it drops to -9dB.
I'm trying to figure out what's the reason for this low bandwidth limit.
--- End quote ---

The leading cause would be the 3 short transmission lines between the resistors and the star point in the middle. Try to eliminate these. The return loss for any port at high frequencies should also be quite bad. A few other things that chop in are the middle pin of the SMA edge connector and the resistors being wider than the 50 Ohm transmission lines, PCB material not made for such high frequencies, probably low quality SMA connectors.

EggertEnjoyer123:
Can you measure the S11 too?
Use smaller resistors and try to stick them as closely together as possible.

Odysseus:
You can also reduce losses by increasing the thickness of your dielectric and/or using microstrip instead of GCPW. This reduces both the dielectric loss with lower field strength and copper losses with reduced current density. This is analogous to using a thicker, lower loss, RF cable. Even though the materials are the same, the loss will improve.

The thicker dielectric has a secondary benefit of a trace width much closer in size to the resistor and connector pads.

Navigation

[0] Message Index

[#] Next page