Some questions about low side RF routing and interconnection

[berger.h]

In the project I need to lead RF (low tens of MHz) with power up to 100W. PCB is only two side FR4 (price) and have some uncertainties and questions. Device is close in full metal case.

1. Impedance + DC resistance.
For my frequency and 1,6mm FR4 is 50Ohm microstrip on about 3mm width of strip.
If on the PCB with such a thick tape do not fit is better to do the whole narrower or where it goes to expand to 3mm?

I have a PCB connection, which at a impedance of 50ohm is a DC resistance, for example, 20uOhm main RF line, straight long. Is it a good idea to solder a wire to reduce the DC resistance (when skineffect is included) to 1/2?

2. RF on Top and on Bottom ground or RF too?
For switching RF signal are on PCB relay (classic mounting, two contacts in parallel)
Two opposing (DIL) contacts are always connected to the relay.
What is better?
Conect RF only on one side and on opposite side spill the ground on on both sides, interconnect the RF.

3.
I need to connect two PCBs that are close together and enclose an angle of 90 degrees. For control signals I use 2x5 2,54mm connector and flat cable.
The question is how to connect a power RF line?
Yes good choice is use coaxial RG316 and any as MCX connector. unfortunately it is a relatively expensive, laborious solution and unnecessarily robust. My PCB are actually touching and it will only bdisassembi in case of failure, That's why I thought.
3mm microstrip on both PCBs terminate on the PCB solder surface and interconnect with a copper strip with a thickness of 0.4 to 0.5mm. For solid groun use for example 5mm wide strip. I think it will have lower losses than the connector.
Is it big stupid?

 

[FvM]

1. Skin depth at the operation frequency is below 35 µ PCB copper plating, increasing the trace thickness is useless. 3 mm microstrip seems appropriate for 100 W, making the trace smaller may result in unacceptable losses.

2. (Almost) continuous ground plane is generally a good idea for RF. Relays qualification for RF must be checked.

3. For SW frequency range, you don't necessarily need coax for PCB interconnect. Regular pin headers arranged for about 50 ohm total impedance can work as well.

 

[volker@muehlhaus]

1. Impedance + DC resistance.
For my frequency and 1,6mm FR4 is 50Ohm microstrip on about 3mm width of strip.
If on the PCB with such a thick tape do not fit is better to do the whole narrower or where it goes to expand to 3mm?

I usually use 2.7mm line width. If you can't keep the line width over the entire length, use it where possible. That is better than using a constant narrow trace width.

2. RF on Top and on Bottom ground or RF too?

The line impedance concept requires that you have proper routing on both signal and ground path. Both are equally important. Ground current must be able to flow directly underneath (or above, for flipped PCB) the signal line. You must never have slots in the ground plane that force RF current to flow a detour, that would create a large series inductance to the entire RF path.

That said, you can have RF trace on the bottom side if you create a proper ground plane on the top side, and both signal and ground can change layer on their natural "direct" way along the signal path. An example how NOT do it: don't use a top side ground that is connected to ground far away from the RF signal path.

3mm microstrip on both PCBs terminate on the PCB solder surface and interconnect with a copper strip with a thickness of 0.4 to 0.5mm. For solid groun use for example 5mm wide strip. I think it will have lower losses than the connector.

If you can keep the line width, that sounds ok. If you can't keep the width, the connection might add a small series inductance, which is not a big deal below 100MHz.

 

[volker@muehlhaus]

An example how NOT do it: don't use a top side ground that is connected to ground far away from the RF signal path.

To avoid misunderdstanding:
don't use a top side ground that is connected ONLY to ground far away from the RF signal path.