Circuit design

The microwave transmitter consists of following blocks:

• Synthesizer (VCO) based on MAX2871 chip and accompanying passives. This guy is able to synthesize frequencies from 25 MHz to 6 GHz. It consists of PLL with integrated VCOs (64 of them). A loop filter (simple low pass RC) is placed externally. This chip actually has 2 differential output ports, but for sake of simplicity I use only one as single ended. All other outputs are terminated with 50 Ω resistors.
• LED that indicates PLL lock detection.
• Teensy (LC or 3.x) that controls the synthesizer over SPI and communicates with a PC via serial port.
• MAX2871 is supplied by 3.3 V, that are scaled down from Teensy's 5V output. Datasheet recommends to use three separate LDOs for each segment of MAX2871 (digital logic, PLL and RF part). It would probably work with only one LDO split in three ways via RF chokes and would be somewhat cheaper, but for the test version I decided to go with recommended three.

Board layout

Layer stackup

For the sake of costs, I managed to squeeze whole design onto a two-layer PCB. I am aware that this is not a recommended approach for a high-frequency design, but it's cheap and possibly worth giving a shot. The PCB, made by OSH Park is a 0.8 mm thick FR408 core, with a dielectric constant of 3.66 at 1GHz.

RF Routing

The most sensitive part of PCB layout are microwave traces. These need to be routed with special care and well shielded. I decided to go for the so called planar waveguide topology on the top layer and used Saturn PCB calculator for dimensioning. Knowing that layer thickness is 0.8 mm, to get 50 Ω line I'd need 1 mm wide conductor with 0.2 mm gap. It is important to have solid non-interrupted return (GND) plane beneath the RF tracks on the bottom layer. I did via stitching at the PCB edge and next to the waveguide to achieve the best possible shielding.

I am not really happy with the way RF has been made (QFN pads very close to each other and routing to SMA connector makes discontinuous trace), but I tried to make the trace as short as possible so, hopefully, the losses won't be that big. I ended up with a 0.25 mm wide and 5 mm long track to the decoupling capacitor and 1.25 mm wide/4 mm long pad of the SMA connector. This definitely isn't 50 Ω transmission line. Simple analysis shows that first line is 85Ω, and second one is 38Ω line. But, luckily, neither is long significant portion of wavelength, even at 6 GHz, maximum is 10% of lambda. Maximum reflection, at 6 GHz, is 0.29, while at some moderately high frequency (2 GHz) it is 0.07.

Power

Expected power consumption is around 200 mA, so power traces are made to be 0.5 mm wide. Power is provided by 5V USB port.