Avian’s Blog

For my tinkering with vector signal measurements I've needed a directional coupler. So far I've been using the "Transverters Store" RF bridge for this purpose. Unfortunately I found it to be less than ideal above 1 GHz. Its design also requires the use of a separate, reference 50 Ω load on a SMA connector, which over time proved to be unreliable and an unnecessary source of problems. I've been wanting to replace it with something better. Mini-Circuits ZHDC-10-63-S seems to be a popular directional coupler with good performance, but it's either perpetually out of stock or not shipping to my part of the world.

I've recently stumbled upon Henrik Forstén's blog. He made his own home brew VNA and generously shared all the design documents, including those for his directional couplers. The directivity measurements he posted show that his couplers are significantly better at high frequencies than what I currently have. He saw better than 25 dB directivity at up to 5.5 GHz. Compare this to the Transverters bridge where directivity falls below 25 dB at around 1 GHz. Making my own copies of his couplers seemed like a straightforward way of improving my measurement setup.

Henrik's coupler design is based on a 2015 IEEE article by Drobotun Nikolay and Mikheev Philipp (at the moment, the paper is freely accessible here). Similar to the Transverters board, the principle of operation is a based on a Wheatstone bridge with a balun made from a coaxial cable and ferrite beads. However the bridge topology as well as the balun design are quite different. This balun uses only one coaxial cable instead of two, and interestingly uses 3 different types of ferrites. The 50 Ω reference is integrated onto the bridge itself. The PCB design uses 4 layers. The coupling factor is 16 dB.

At first I thought getting the PCB made would be as simple as zipping up Henrik's Gerber files and sending them off to AISLER. Unfortunately that didn't work out. As much as I fiddled with the Gerber files I couldn't get the AISLER's on-line ordering system to accept them. I tried deleting the "CUTOUT" letters on the board outline layer and it didn't help. In the end it might have been the fact that the board is slightly narrower than the 15 mm minimum.

I ended up redrawing the whole thing in a PCB design program that-shall-not-be-named and making a fresh new set of Gerbers. In the end I think that turned out for the best, because it made me look a bit deeper into this design and do a few modifications.

Henrik had his PCBs made using OSH Park 4 layer service. This process uses a high-frequency, low permeability substrate FR408. My AISLER boards will be made with the 4-Layer HD stackup which uses just plain old FR-4. So when redrawing the designs it occurred to me to also adjust trace widths so that characteristic impedances would stay the same.

One thing I could not figure out were these narrowed sections of the traces around the bridge section. The wider part of the trace is approximately 50 Ω based on OSH Park's process parameters. The narrower part is closer to 75 Ω. I'm not sure why the narrow part is necessary. I can't see it in the figures in the original IEEE article either, although authors don't provide a good picture of the final design so it's hard to say.

The only reason I can think of is thermal relief, to avoid the SMA connectors from sinking too much heat when soldering the resistors and the balun. Since the whole divider part is only around 4 mm across I doubt trace impedances play much role in signal integrity. 1/10 wavelength rule gives a maximum frequency of around 4 GHz for traces without a controlled impedance.

Image by Drobotun Nikolay and Mikheev Philipp (modified)

Where the traces meet the SMA connectors they need to be widened so that the connector pin lands properly. The IEEE article mentions using microstrip tapers for better matching in this part. Henrik's design doesn't use these, however it keeps the connector center pin footprint at about 50 Ω by dropping the ground plane by one layer beneath the footprint.

Another difference I found between the paper and Henrik's design were the resistor values. The paper mentions that the resistor next to the balun needs to be about 10% larger (10.3 Ω) than the theoretical value (9.3 Ω) due to some unspecified effect of the balun. Henrik lists the uncorrected value in his BOM.

Another thing to note about the resistors is that the pads on the PCB fit tiny 0402 size packages. I suspect these will be quite a challenge to solder manually, especially since they're very close to where the coaxial cable lands. Actually, the whole coupler is just 40 x 15 mm - much smaller than it appears on the photos.

In my modified design I've re-calculated all the trace widths to 50 Ω at AISLER's process parameters and left out the narrowed sections. I also slightly enlarged to board so that it's now exactly 15 mm wide and made sure that it complies with the 0.3 mm edge clearance design rule. I was tempted to switch to larger 0603 resistors, but I'm guessing these come with worse high-frequency response as well, so I left them at 0402. In the end I also added some helpful labels on the silkscreen print layer.

Now I'm waiting for the PCBs to be delivered. Thankfully I didn't have any problems ordering the exact ferrite types. Again I'm really grateful that Henrik went through the trouble of documenting his instrument and publishing the designs. We'll see how well my copies perform. After I assemble one and check that it works reasonably well I plan to also publish my modified Gerbers and BOM for anyone else that wants to make a copy of these devices using a FR-4 process.