I've been working on a 4-layer design built around the EFR32BG13 Bluetooth Low Energy SoC. While trying to measure the impedance of the antenna to build a matching circuit, I discovered that my short grounded coplanar waveguide (GCPW) transmission line was acting more like an antenna than a transmission line.
To narrow down the cause of the issue, I built a simple 4-layer transmission line test board, which is pictured here:
The board is 100 mm square. I had these boards fabricated by ALLPCB, who specify 35 μm copper on all layers and 0.175 mm dielectric (dielectric constant 4.29) between the first two layers. Using AppCAD, I found that a design with 0.35 mm trace width and 0.25 mm gap yields an impedance of 48.5 Ω. The top layer for the board is shown in red above. The other three layers are ground planes that look like this:
I received the boards today and began by testing S21 for the second section from the bottom--a straight piece of GCPW with SMA connectors on either end. I used an HP 8753C / HP 85047A with a short length of coax connected to Ports 1 and 2 and the test board connected between those lengths of coax. Much to my surprise, this is what I saw:
At 2.45 GHz, my transmission line has a response of -10 dB. If I replace the board with a "thru" connector, I see exactly what I would expect:
I'm at a bit of a loss, as I thought that the first test would be a slam dunk and I would start finding issues with the more complex tests above it. I have a VNA and a strong desire to learn what I'm doing wrong here. Can you see any problems with my testing method or with the GCPW design itself? Any help at all would be greatly appreciated!
Edit: As suggested by Neil_UK, I have removed the thermals on one board by scraping away solder mask and then bridging the gap with solder. Measuring S11 and S21 with this configuration gives the following result:
Comparing the S21 plot with the previous result, there does not seem to be any perceptible difference.
Edit 2: As suggested by mkeith, I have split one of the "strips" of my test board apart from the rest using the old "score and break" method. The board I chose to break off is the same board I removed thermals on, so this result is a further modification on the preceding plot. Here it is:
There is a deepening of the troughs in the S11 plot, but no significant improvement in the board's functionality as a transmission line.
Edit 3: Here is a photo of the board in its most recent embodiment:
Edit 4: Close-up shots of both sides of one SMA connector:
The SMA connector is Molex 0732511150. The PCB land follows the recommendations in the datasheet here:
Edit 5: Here is a cross-section of the board near one edge:
The green lines are scaled from the manufacturer's specifications, which are copied here:
Edit 6: Here is a top-down photo of the board with red scale lines showing the expected dimensions:
Edit 7: To verify the effect of the large center SMA land, I carved away the central pad on one board so that it was the same width as the rest of the trace. Then I used copper tape to extend the grounds on either side:
Then I retested S11 and S21:
This seems to have improved S11 significantly, which leads me to believe that the large center land was, in fact, creating a capacitance at either end of the line resulting in resonance.
Edit 8: Looking for some guidance on how to handle the transition from SMA to GCPW, I came across this white paper:
While the paper specifically refers to the use of a high frequency substrate, I think much of it is still applicable here. Two main points stand out for me:
- The GCPW should continue all the way to the edge of the board.
- High frequency end launch SMA connectors use a center pin that is shorter and narrower to minimize its effect on the GCPW. These may be more appropriate for an application like this with a thin central conductor on the transmission line.