RF board layout

The wavelength at 2 GHz, even in a pcb trace, is inches. So a surface-mount pad is not significant from an impedance discontinuity standpoint. Short traces won't matter much either.

On faster stuff, we sometimes punch a hole in the layer 2 ground plane, to reduce pad capacitance, which we do mostly by guesswork.

It's worth analyzing vias if they are in your signal path. A common via might add a full pF or more.

I assume that layer 2 is your ground plane, and the board is FR4. How thick is your first dielectric layer? Some pcb houses default to absurd thicknesses like 4 mils, and don't read fab drawings.

the schematic, all are in SMT packages - fully internally matched to 50 Ohm amplifiers, bias-T, AC coupling 0402 capacitors, fixed attenuators, progra mmable attenuators, filters, RF switches. All components are declared in th eir data sheet as designed for 50 Ohm system and they are also tested that way.

ake all pads and traces to be 50 Ohm.

ted by manufacturers: 12, 14, 24, 31, 42, 60 mil.

can't be of the same characteristic impedance. It is simply because of thei r different width.

The material is Isola FR408, L2 is a reference ground layers, Top to L2 die lectric thickness is 5.8 mil, epsilon is 3.8.

There are only power supply voltage and ground vias, all routing is done on the top layer.

So a 12 mil wide trace is 50 ohms. That's why the pads seem so huge.

A 10-layer board, also in process now, will be 8 mils from L1 to L2 ground, for a 14 mil 50 ohm trace. Inner layers traces need to be 6 mils.

Theoretically you could adapt by etching away part of the ground plane underneath pads that are wider than 50ohms would allow, or if too small add top ground traces very close to them to bring the impedance down. However, as John wrote, at 2GHz short sections such as pads don't matter much.

Here's a bit of analog stuff that works at about 1.5 GHz

I used a lot of vias and sideways caps to get good grounding and bypassing. L2 is solid ground and L3 has power pours.

he schematic, all are in SMT packages - fully internally matched to 50 Ohm amplifiers, bias-T, AC coupling 0402 capacitors, fixed attenuators, program mable attenuators, filters, RF switches. All components are declared in the ir data sheet as designed for 50 Ohm system and they are also tested that w ay.

ke all pads and traces to be 50 Ohm.

ed by manufacturers: 12, 14, 24, 31, 42, 60 mil.

an't be of the same characteristic impedance. It is simply because of their different width.

You?ll want to choose a polyamide PCB like GETEK or equiv for bette r loss tangent.. Thinner dielectrics allow finer trace 50 ohm traces. But depends if you wanta Return loss of 15 dB or better. Use Saturn PCB design tools (free) Electrical impedance testing is suggested or specified.

Hello, It was lovely. Thank you to everybody who took a moment and participated. I am grateful for your quick help. Keep safe and healthy. Sincerely

So hang out and help other folks. All kinds of folks are here, as you can instantly see. ;)

Cheers

Phil Hobbs

he schematic, all are in SMT packages - fully internally matched to 50 Ohm amplifiers, bias-T, AC coupling 0402 capacitors, fixed attenuators, program mable attenuators, filters, RF switches. All components are declared in the ir data sheet as designed for 50 Ohm system and they are also tested that w ay.

ke all pads and traces to be 50 Ohm.

ed by manufacturers: 12, 14, 24, 31, 42, 60 mil.

an't be of the same characteristic impedance. It is simply because of their different width.

Use Duriod and co-planer microstrip. (maybe not that critical at 2Ghz) We h ad a board built for 8Ghz, it was a disaster. The company used FR4, too muc h loss, should have been Duroid. They used 50 ohm lines, but should have be en co-planer microstrip, but wasn't. The microstrip radiates and ba modes e xist without co-planer. With the two losses, we couldn't get the required output power.